Mazak T-Plus Eia/Iso (G-Code) Programming Questions

Howdy Everyone,

I'm making strides in getting my mid 1990's vintage Mazak QT-20N running. I am, however a bit stumped with Mazatrol. Everything I've read seems to indicate that programming on the machine using this control is quite easy. Trouble is, I'm still scratching my head after playing around with it for a few days. I have a fairly decent understanding of G-code and have used it in the past to program my other machines. Plus, I've been using BobCad V26 for a while to design parts, generate tool paths and post code. At this point I have all my tooling, cutting parameters and, most importantly, over 100 parts already drawn in BobCad and ready to be exported to this machine. As such, I'm having a hard time justifying the time and effort it would take to replicate all of this at the machine using Mazatrol T-Plus. It seems to me my time would be better served simply posting my existing G-code in a format that can be read by Mazatrol and loading it into the machine. I have been playing around with the machine and do have the option of writing a program in eia/iso mode. My understanding is that this is simply another name for G-code. I've posted the code for a very simple part that I've run 1000's of times on other machines. I've noted the questions I have below the code.

%
O00100 ( PROGRAM NUMBER )
( PROGRAM START - TURNING CYCLES )
( PROGRAM NAME: 1.NC)
( POST: MAZATROL T32 REV2)
( DATE: TUE. 02/17/2015)
( TIME: 02:26PM)
(Machine Setup - 1 Face Basic Finish )
(TOOL #3 Roughing )
N01 G53.5
N02 G28 U0. W0.
N03 T0303
N04 G50 S2000
N05 G96 S500 M03
N06 G00 X.75 Z.25 M08
N07 G01 X.5 Z0. F.015
N08 X0.
N09 X-.125
N10 G00 Z5.
N11 X5.
N12 G00 G28 U0. W0.
N13 M01
(Machine Setup - 1 Turn Rough )
(TOOL #1 Finishing )
N14 G53.5
N15 G28 U0. W0.
N16 T0101
N17 G50 S2000
N18 G96 S500 M03
N19 G00 X.6 Z.1 M08
N20 X.4
N21 G01 Z-.7397 F.015
N22 X.4727 Z-.7399
N23 G03 X.4989 Z-.7616 I-.0021 K-.0292
N24 G01 X.5 Z-.7725
N25 Z-2.985
N26 G00 Z.1
N27 X.3711
N28 G01 Z0.
N29 G03 X.384 Z-.031 I-.033 K-.032
N30 G01 Z-.7397
N31 X.4
N32 G00 X.484
N33 Z-.5816
N34 G01 X.384
N35 G01 Z-.6816
N36 G03 X.3825 Z-.7035 I-.07 K-.0064
N37 G01 X.3803 Z-.7085
N38 X.3609 Z-.7397
N39 X.384
N40 G00 X2.
N41 Z2.
(Machine Setup - 1 Turn Basic Finish )
(TOOL #1 Finishing )
N42 G00 G54 G97 S62 T0101
N43 G50 S2000
N44 G96 S500
N45 G00 X.6 Z.1
N46 X.3443
N47 G01 Z0. F.015
N48 G03 X.3733 Z-.026 I-.0016 K-.031
N49 G01 X.374 Z-.1487
N50 Z-.689
N51 G03 X.372 Z-.7029 I-.0279 K-.003
N52 G01 X.3457 Z-.7452
N53 G02 X.3576 Z-.7497 I.0121 K.0141
N54 G01 X.472 Z-.7498
N55 G03 X.4898 Z-.768 I-.0015 K-.0193
N56 G01 X.49 Z-2.785
N57 Z-2.985
N58 G00 X2.
N59 Z2.
N60 G00 G28 U0. W0.
N61 M01
(Machine Setup - 1 Cutoff )
(TOOL #11 Parting )
N62 G53.5
N63 G28 U0. W0.
N64 T1111
N65 G50 S1000
N66 G96 S500 M03
N67 G00 X.6 Z-3.259 M08
N68 G01 X0. Z0. F.015
N69 G00 X0. Z0.
N70 G01 X.3 Z-3.259
N71 G00 X.5
N72 G01 X.1
N73 G00 X.3
N74 G01 X0.
N75 G00 X5.
N76 Z5.
N77 G28 U0. W0.
N78 M30
%

1) You'll notice this post is in Mazatrol T32 format. I can have a custom post written by BobCad for T-Plus. I'm happy to spend the money to do this, however BobCad can't even tell me if they have written a post for this control. Is anyone using a BobCad post for mazatrol T-Plus? Is there really "that" much difference between the code above and that required for T-Plus? I mean... it's G-code, there can't be too many differences.

2) To coincide with the question above. I've got a full set of manuals for the machine but don't have a manual that is specific to eia/iso programming? Does such a beast even exist?

3) Included in the manuals is an M-Code list but no G-Code list. Anyone know of a location of such a list for this control?

4) I've used the tool eye to set the locations for the 3 tools called out in the above program (rough, finish & parting). I have also used the tool library in Mazatrol to setup tool radius and angles. With my past experience on fanuc machines, tool offsets would be based off one "master" tool. The offsets for the remaining tools in the turret would be based off the difference in X & Z locations of each of those tools compared to the master tool. When running a program each tool would be called up as T0101 (tool one, offset one), T0202 (tool two offset two), etc... With Mazatrol and the tool eye, though, I'm getting impression that tool offsets are a bit different. Since the location of each tool is stored in the control based upon the tool eye, does the offset for each tool need to be called input somewhere else in the tool library? I'm under the assumption that when calling up T0101 or T0303 etc.. the control automatically associated offset 03 as being associated with the measurements produced by tool number 03 when it was measured by the tool eye.

5) With past machines, to set the program Z zero point I'd home the machine and call up my master tool (T0101) and touch it to the end of the work piece being machined. I'd zero out the display and send the machine by home. The distance traveled would then be my work piece zero. This data would be entered at the top of the program with a G50 X0.0 Z5.360 (or whatever that distance was). With the T-plus control where the heck do I enter this data in the program?

ben_smith said:

I'm having a hard time justifying the time and effort it would take to replicate all of this at the machine using Mazatrol T-Plus. It seems to me my time would be better served simply posting my existing G-code in a format that can be read by Mazatrol and loading it into the machine.

Click to expand...

Yes and no. G-Code sucks. It's like refusing to upgrade to a Windows (Icon driven) format because you are comfortable with DOS.

Tool wear offsets will be controlled in a different page with G-Code program vs on the geometry page. The T+ will ignore any wear offsets entered there for G-Code programs. The only reason I know this is the old farts who ran the Integrex after me REFUSED to run the Mazatrol programs I created and insisted the programers made them 'official' G-Code programs.

They had a lot more fuckups because they got rid of the graphical interface and just relied on the 'distance to go' screen they knew and loved.

Post up a hand drawn sketch of the above part and I will program it in Mazatrol (on an old ass 1986 T-3 controller) and take a screen shot for you.

Boy, that would be great. I've attached a drawing of this pin. Material is 6061 Aluminum. I typically produce these in two operations. Face and turn the OD then part a bit longer than finished size. Second operation, flip the pin over in the chuck and face to final length. Typically this would be a bar feeder or bar puller job, spitting out a few hundred a day. Right now I'd just settle for getting one pin programmed and run out. I'm quite comfortable using BobCad to design all my parts and spit out the code. I would just like to be able to get this machine to work with this process. On my old Okuma, I could have this part loaded and running in just a few minutes. I'd like to get to that point with the Mazak.

Once you are familiar with Mazatrol, you can write that program in less than 3 minutes. Mazatrol is great for simple stuff, not so great for complex shapes.
Why not just part to length? I'm not familiar with your tolerancing. Please educate me.

ben_smith said:

Boy, that would be great. I've attached a drawing of this pin. Material is 6061 Aluminum. I typically produce these in two operations. Face and turn the OD then part a bit longer than finished size. Second operation, flip the pin over in the chuck and face to final length. Typically this would be a bar feeder or bar puller job, spitting out a few hundred a day.

Click to expand...

Sorry I forgot about this yesterday. I will post the screen shot tonight.

The code you posted does not look anything like the example. Am I missing something?

Gobo,
The top of the pin (i.e. the tip of the larger diameter section) needs to be smooth. The finish from parting just isn't as good as I need.

Phil,
Thanks a bunch! The code posted above is indeed the post for the pin in Mazak T32 as processed by my BobCad program. It looks very similar to the posting I used to run on the Okuma. It still needs edited a bit to reduce a few unnecessary movements... but I just wanted to export something to get a part made.

From everything I've read online, using Mazatrol to program at the machine is significantly better than using Cad/Cam, posting g-code and uploading to the machine. Since I'm used to drawing my part and producing my tool paths in Bobcad and then sending them to the machine, I'm just having a hard time figuring out how to transition into the Mazatrol process. I'm following the manuals but still can't wrap my head around the interface on the machine.

ben_smith said:

I'm just having a hard time figuring out how to transition into the Mazatrol process. I'm following the manuals but still can't wrap my head around the interface on the machine.

Click to expand...

Honestly, the absolute best way to learn Mazatrol is having someone knowledgeable stand there at the machine with you for 2 days while you learn and ask questions. This is the training Mazak provided us when we inherited an old QT10N from another division back in 1995. The applications engineer said, "I showed you about 40% of what this machine can do. The rest you will pick up as you go." He was right.

Funny part is that machine is my pride and joy. Been running the old POS for 18 years now and I still love it.

ben_smith said:

The code posted above is indeed the post for the pin in Mazak T32 as processed by my BobCad program.

Click to expand...

I still do not follow how the X numbers jive with the part you posted. Perhaps Bobcad post is using radius offset instead of diameter?

Regardless, here are the screen shots as promised. The final process is the bar pull operation (MNP), which is still a "G-code" type of format, but in a grid fashion similar to Microsoft Excel. You just enter the values as needed in the correct column and the machine handles the rest. Notice how it does not have any information on spindle direction, coolant, tool, etc, just very basic info.

Also, make sure you look at the END process. This process is VERY POWERFUL in Mazatrol. You can see I enabled the parts counter and also looped the program to run 9 times and then shut off, assuming the bars are 30" or so long.

Anyway, it took WAY longer to actually write this post vs program the machine if that gives you any indication of the speed in which the machine can be programmed.

Tool 9 = CNMG 432
Tool 10 = VNGP 332
Tool 3 = .125" part off tool / Royal bar puller combo

The G code in post # 1 is NOT for Mazak EIA, regardless of what Bob said it was giving you. Mazak usually hides their lists of G and M codes somewhere in the middle of their manuals, and do not even list them in the contents / index, you have to search for them. Much easier as you can see from Philibuster's post to spend a couple hours with someone who knows Mazatrol to show you the basics. You will be RUNNING your mazatrol program before you can even draw your part in B Cad.

You should invest in some training for Mazatrol. You will love how quick you can get a part running production.
You will ditch the G-code for turning.

Thanks Guys!

I'm able to get some basic parts running. The biggest difference I've noticed thus far is that X & Z are positive values as I move towards the chuck. With my Okuma and g-code these are negative values. I'll give Mazatrol and honest try before I reconsider using BobCad to load code into the machine. A couple questions, though:

1) When facing I typically like to move the tool about .050 past the X center line. Mazatrol will only let me move a facing tool to x0.0 and not beyond. What am I missing here?

2) The small .035" radius groove in the above pin is giving me fits in Mazatrol. This is easy with my Cad/Cam software, but I can't figure it out in Mazatrol. Any thoughts?

3) My tool eye calibration is seriously off in the X axis. The values calculated by the tool eye are 7.3227" off actual X axis center. I was perplexed when my tools wandered waaaaay off centerline until I set the X offset by turning a piece of stock, measuring the OD and using the teach function. Is the any way to adjust the tool eye to reflect actual X centerline?

ben_smith said:

1) When facing I typically like to move the tool about .050 past the X center line. Mazatrol will only let me move a facing tool to x0.0 and not beyond. What am I missing here?

Click to expand...

If your tool data for your facing tool has the correct nose radius entered, Mazatrol will drive the tool that much past your center line. You enter the nose radius by going to your TOOL DATA page No. 2. found on the far right of your tool data page.
It sounds like your tool eye is seriously out of calibration, though I cant imagine why so much. There is a simple process for calibration found in the manual.

ben_smith said:

Thanks Guys!

I'm able to get some basic parts running. The biggest difference I've noticed thus far is that X & Z are positive values as I move towards the chuck. With my Okuma and g-code these are negative values. I'll give Mazatrol and honest try before I reconsider using BobCad to load code into the machine. A couple questions, though:

1) When facing I typically like to move the tool about .050 past the X center line. Mazatrol will only let me move a facing tool to x0.0 and not beyond. What am I missing here?

2) The small .035" radius groove in the above pin is giving me fits in Mazatrol. This is easy with my Cad/Cam software, but I can't figure it out in Mazatrol. Any thoughts?

3) My tool eye calibration is seriously off in the X axis. The values calculated by the tool eye are 7.3227" off actual X axis center. I was perplexed when my tools wandered waaaaay off centerline until I set the X offset by turning a piece of stock, measuring the OD and using the teach function. Is the any way to adjust the tool eye to reflect actual X centerline?

Click to expand...

Mazatrol uses the end face as the part zero. The Z values are positive when programming in Mazatrol to eliminate the need to put in a negative sign all the time. The only processes that use positive values to the right side of zero is EDG and MNP.

When you push cycle start and run the program, you will see the Z values displayed on the screen are indeed negative values per normal.

1) Facing on Mazatrol past center can only be done with the EDG process. The machine will drive the tool to a -X value exactly 2x the radius value in the tool file. Change the insert radius and the machine will compensate. The tool file must reflect the tool, meaning cutting angles and tip radius and chuck direction. If you get this wrong, the machine does not know how to comp the tool path. VERY IMPORTANT.

2) Sorry about that. I forgot the automatic undercut I put in my program is controlled by the individual machine's USER parameters. Look in your T+ programming book to see which values to change. The user parameters for my old T-3 machine for a #1 undercut are controlled by U9 (length of undercut--set to 500) and U10 (radial depth--set to 320). Mazak calls this a grind relief in the manual.

Anytime I want to create an undercut for a VNGP332, I just poke a #1 undercut. I use #5 undercut for a VNGP331 insert (U11=400, U12=160).

You can create the undercut with part geometry, but the machine is smart, meaning if the roughing tool will not "fit" in there, it will not drive the finisher tool in there either, except only to remove the stock allowance specified in PNo0. Nice feature for sure. You can however get around this by copying the process and putting a rough only tool on one process and a finish only tool on the second copied process. Use caution of course.

3) The manual will have the tool probe calibration parameters to adjust. Always check the headstock for taper FIRST before you adjust the probe, otherwise you have to do it all over again. Calibrate the OD tool probe button first. ID tools are just an incremental value from the OD button (on the T-3 anyway). You will chase your tail if you calibrate the ID first.

What he said up there ^

The one thing you have to remember with Mazatrol...

You aren't programming the machine the way you would with a CAM program...

You are describing the geometry of the part, the machine takes care of the rest...

You will, I guarantee it, I've seen it a bunch, think that you are smarter than the machine and try lying to it... You seldom have
to lie to it.. Just keep telling yourself that you are telling the machine what the part (or feature) looks like, give her some feeds
speeds and DOC's and she'll 99% of the time figure it out for you.

I could have made 2 Mazatrol programs, straight from the print in the time it took me to type this post.

Bobw said:

The one thing you have to remember with Mazatrol...

You are describing the geometry of the part, the machine takes care of the rest...

Click to expand...

This cannot be over emphasized. Thanks for the simple short explanation. I got a little too wordy...

Thanks Everyone!!

I've got the beast spitting out parts like crazy. Mazatrol does seem to be fairly easy.... once you understand how to "talk" to it. Holding a .0002" tolerance all day long.

Any questions free feel to ask.

I had three QT20's at one time with barfeeds and parts catchers....It never ceases to amaze me how quick a guy can run parts through those machines and how accurate they were. When it comes to 2 axis turning, nothing beats a Mazak.

Two videos attached to this thread.

http://www.practicalmachinist.com/vb/mazak/any-mazatrol-videos-285483/

I know this post a few years old, but I'm gonna try bumping it.

Lots of good info here, really helpful since I've programmed g-code and only just got a Mazak QT18 NSP and trying to learn Mazatrol T32-2.

Can any of you wizards post a screenshot of how a bar change program in mazatrol should look. I'm struggling with it in g-code, but would really want it as mazatrol if possible. I have FMB turbo LMS bar feeder attached. The machine had no bar change or top cut progrrams in it when I got it. M68 is Cycle Bar feed call 1 and M69 is Cycle Bar feed call 2.