[fpworks]

Bear with me, I am completely ignorant with regards to Mazatrol.

We are buying a new VMC this spring and the new Mazaks are shipping with the new Mazatrol Matrix controller. As we narrow down the choices, the Mazaks looks real good, but I've always heard very strong mixed opinions with regards to Mazak controllers.

To help our purchasing decision, I need to know: Do Mazak controls have any issues with ISO standard G-code? (in terms of compatibility and block execution speed, or anything else I should know about)

It is desireable for whatever machine we buy to handle our existing Fanuc programs (some minor modification/editing is expected) This machine will not be doing any conversational or at-the-machine programming. (except for program adjustments)

Thanks for any insight.

Justin

[psychomill]

Yes, the Mazak controls handle the g-codes just fine. As a matter of fact, I only program mills in g-code and don't use the Mazatrol side, not even for probing, Tool break check, etc. There are some things on the Mazatrol side you may want to use however like tool life, max spindle speed (on the tool), slow tool change, HP limits, etc.

As far as block execution speed,.... Mazatrol is extremely fast. You won't be dissappointed with it in that regards.

A few things to consider... Not sure of what options you're looking into or getting for the machine, but the following are definately worth considering....

2D Shape contour (2D High speed machining software... also called MAZACC 2D)
MAZACC 3D (if you do a lot of 3D machining)
EIA Probing software (if you plan on using a machine probe)
EIA Tool break Check Sub routines ( for G code TBC cycles)
Extended workoffsets and 600 set Macro variables, macro B
Extended tool offsetting

There's a host of other stuff too so really look into this...

Tornado Bore, Spline interpolation, Nurb interpolation, Hi-pressure thru spindle coolant (1000psi), different conveyor setups, spiral interpolation (similar to G12/13 but with capability of 3D, "screw" type apps, full pocketing, etc), then other control options like IC card slots (I think this is standard), Floppy drive, all the different ethernet stuff... etc.

[fpworks]

Great, thanks for the information. Some of those features look very promising. You just gave me a lot more to think about in terms of control options. I'll take a look at those.

We're looking at the VCN 410BII or 510CII. Still up in the air over getting a 'HS' version or adding a 4th with an indexer subsystem.

There is a lot of competition for this type/size of machine, and it seems the only thing that sets them apart (on paper) is the controls and service.

Justin

[MDLang]

VCN 410BII or 510CII.

fpworks,

At the shop that I currently work at we have a Nexus 510C. Very fast tool changes and nice rapid rates. The fully enclosed workspace is nice as well, but. I've come to really dislike the the table moving on both the X and Y. We have three varieties of Mazak mill representing three varieties of table movement. X only table and Y,Z on the column(V515). X,Y on the table and Z on the column(510C) and Stationary table with X,Y and Z on the column(Vtc 200B).

At first the 510C was my favorite But after some time on the other two types the Vtc 200B has come out as my preference over the 510C. The V515 is a different class of machine.

With a 510 if you wish to check your inserts you need to remove the tool from the spindle or lean way into the machine to have a look as you can't bring the tool to you(the column only moves on the Z).

Although the 510C has very fast tool changes it needs to move all three axis to a safe tool change position, likely moving the table near full stroke away from home. This slows the tool change process somewhat and really increases axis movement over a days production. The Vtc 200 will only return the column to tool change position on the Y and Z axis regardless of where it is on the X. The 510 is still faster thought.

Another pesky feature of the 510C is the fact that the part to be machined is moved away from you when you start to machine it so it can be difficult to watch for clearance issues and see what's going on during first offs. If you ever hang parts off the table you need to remember that can't be done as the table on a 510 comes close contact with all sides of its enclosure.

With the Vtc200 the part stays right in front of you. It has a larger table making it easier to leave a 4th mounted on the table and still run two or three vices. It may be a quirk of the machine we have but both of our Vtc's have better rigidity than the 510 and the 200 is easier to service.

A 510 and the Vtc's share the same spindle, have the same horsepower ratings and both come in either a 40 or 50 taper so unless shop floor space is a consideration a Vtc is a more versitile servicable and rigid machine. Only real drawback other than larger space requirement is the open top enclosure can create some rain when drilling with throught coolant drills.

If you are machining lots of little parts with lots of rapid moves, tool changes, part changes and low demands for table space then get a 410 if you need the 510's table then have a look at the Vtc's, They are a good machine

Just thought I'd share my opinion with you.

[fpworks]

MDLang,
Thanks for the information. I appreciate that kind of operator-specific feedback.

I think it is weird that a c-frame machine must go to a specific x-y position for a toolchange since the spindle is stationary in x and y. Can that be disabled with a parameter change?

Good points about part visibility. I never really gave it much thought since all I've ever used is c-frame machines. I'll go ahead and get some quotes for some of the other Mazak VMC configurations, since we are also looking at y-z column (table moves x only) Okumas as well.

Justin

[MDLang]

fpworks,

Our 510 has a renishaw lazer tool setter, very nice but, there is an arm that sticks up something like 10 inches at the left rear corner of the table. The only safe tool change position is near full stroke away from home so that long tools swing just to the inside of the arm as the come into the spindle.

We set it this way as the change position is fully adjustable by the user. It's important to remember that the ATC arm will drop the tool out of the spindle several inches before it swings. 5 inches clearance from your longest tool to a fixture, touch setter or work piece is now a hit on a tool change. They used to let it change above work piece untill one day they had a 1.25 insert drill take the head off the lazer tool setter. Very expensive little part to replace.

You could change it according to what your running but mistakes will happen so we've set it in an allways safe position.

We are a 10 machine shop, all Mazak except for one Mori lathe. For those 1 - 50 part runs that you may never see again I can't imagine anything getting you cutting faster than mazatrol. After that the short comings of the mazatrol system start to become appearant. There is a parameter for almost everything but unless you are dedicating the machine to a very long part run it's not safe to change some of the parameters to improve cycle time. If you forget to reset a clearance setting for the next job you may have a problem.

We do almost exclusively oilfield work in short but repetitive runs. Over time we have started using more and more g-code subs to improve cycle times. It's the only way to effectively get around "tool path abuse" generated by the conversational controll. I have a handy program called Camlink by Griffo Bros. so I can take a g-code sub and convert it into a Mazatrol manual unit (g-code program that runs as a single unit within a Mazatrol program). Only problem is that a Mazatrol program can only be 200 lines long so you need to start nesting Mazatrol subs within Mazatrol subs. The advantage is that your mazatrol g-code unit will pick up any mazatrol offsets were as an EIA sub will not.

If you do a lot of pocket milling with feed mills (I love feedmills) there is no unit for ramping into the cut with the fusion controll but I think the Matrix controll will do it. If you want to spiral or conical mill you need to do it as a g-code sub and there is no unit for helical milling around something like a trunnion so thats a g-code sub as well.

I'm blabbering on now so to sum up If you do long part runs with slightly more complex geometry and don't create alot of new programs then I don't think you need a Mazak, an Okuma is probably a better choice.

If you do short part runs repeating or not and create alot of new programs complex or not and especially if they require 4th axis work then Mazatrol makes that a breeze and the less than efficient tool paths don't matter because the time you saved programming will far exceed and time wasted during machining.

Just make sure you have probing capability, high pressure through coolant and see if they have come up with air through the spindle yet for those feedmill jobs.

Good luck, our next mill may not be a mazak.

Mike

[Dean0017]

Hey guy's, if you're using EIA/ISO programming, you should be able to tool change by only moving home on the z-axis. (G28 Z.0) then T?M6.

If your code looks like this it will home on all axis before tool change.

G28 X.0 Y.0
G28 Z.0
T?M6

Just remove the first line and you should be golden.

For Mazatrol, I'm not sure. Maybe contact your local mazak profesional.

OH! one other note. If you don't like the way the Matrix control handles tool offsets this can all be changed. Sometimes form factory the controler does not hand offsets similar to Fanuc. But with a few parameter changes it can. Just never underestimate this controler.

Dean

[MrMazak]

G28 X0.0 Y0.0 Z0.0 will move the tool to the part 0.0 position (likely a crash)

G28 (or G30 HOME#2 pos) G91 Z0.0
G28 G91 Y0.0
T01
M06

Go here http://www.cncci.com/resources/tips/...28%20works.htm

Here is a program from my FH5800
(======= START OF PROGRAM =======)
N100 G20
N102 G0 G95 G17 G40 G80 G90
( 3/4 FLAT ENDMILL TOOL20 DIA .750 )
N103 G30 G91 Z0.0
N104 G30 G91 Y0.0
N104 T22
N106 M6
N108 T1
N110 S3000 M3
N112 G0 G90 G54 X7.175 Y1.1498
N114 Z3.0 M8
N116 Z2.388
N118 G1 Z1.05 F.010
N120 Y.8998 F.005
blah
blah
blah
N176 Y-.6498 F.004
N178 Y-.8998 F.009
N180 Y-1.1498 F.005
N182 Z1.1
N184 G0 Z3.
N186 M5
N188 G91 G30 Z0.
N189 G91 G30 Y0.
N190 M01
( 3/4 BALL ENDMILL TOOL1 DIA .750 )
( TOP SIDE ROUGH )
N192 T1
N194 M6
N196 T26
N198 S5000 M3
N200 G0 G90 G54 X6.1825 Y-.8734
blah
blah