mazak matrix nexus control

[TREV]

good evening all,

its been a real long time since I popped in here and here it goes:

we just received a new Mazak 530c hs machine with a matrix nexus control.

I have never run a mazatrol control before so I have a question regaeding the post.

I am starting with the mpmaster versus taking one of my existing and altering it. I am more of a fanuc

fan but this is what we got. i'll not make any judgments at this time.

so is there anything I need to look for right out of the gate? or will I be ok for starting out with out making changes?

I realize as time goes by I will most likely alter to more of my liking however the sooner I get up and running

without all the bells and whisles right now is all well and good.

 

another thing I noticed in some older threads was the discussion on tool offset versus tool data.

I have a laser and probe in this so all tool measuring will be done on laser. it seemed that tool data was preferred by more Mazak fans versus those more used to fanuc controls. any more thoughts on this.

 

thank you,

trevor

[Zoffen]

Mazaks usually (check parameters to confirm) use the tool call, ie T1 M6, to apply tool height so no need for g43.

I use the mazak tool length in the tool data page.

 

Other than that works mostly like fanucs except for the highspeed stuff (G61.1).

 

I started with mpmasters and with few mods was making chips.

 

Good luck!

[TREV]

Zach,

 

I will be usung this machine for mold work so what im curious about in regards to high speed is this

have you noticed the g64 will "overshoot" geometry and how much does g61.1 slow down the control.

basicly should I use g64 for roughing and g61.1 for finishing? also I was seeing some mention of a K

value to correspond with g61.1 . as K70 being the default and a lower K value more accurate.

what is your experience with this?

trevor

[Joe788]

Trevor, it all depends on how the parameters are set as far as whether or not you use the Tool Data or Tool Offset page, as well as the H calls for the tools. I had all Fanuc controls before switching to Mazak, so mine are all set up to use G43H just like any Fanuc machine. You can take your program right out of one of your existing machines, put it in the Mazak, and the only thing you'd need to change is the high speed commands, maybe some coolant thru M codes, and rigid tap M codes. (I have the parameters on all mine set to rigid tap automatically on G84, so there is no M code at all).

 

I use the Tool Data page for the tool length only. The wear comp for the length and diameter come from the Tool Offset page. This is handy, because if you have the wrong H number on your G43 line, the machine will still use the tool length of the tool that's actually in the spindle, and will use the wear comp of the incorrect H number. So worst case scenario, your length is only off a few thou.

 

You're probably not going to be happy making molds if all you have is G61.1. That's MAZACC2D - for lines and arcs. It doesn't like splines. You should have them come out and upgrade you to MAZACC3D at the minimum. I think it costs $3500. It's actual additional hardware that gets installed in the control. Since you're primarily making molds though, you might want to get "fine spline interpolation" and "high smoothing control" too. That's another $5K on top of MAZACC3D, but you'll be fully decked out at that point.

 

I believe the latest version of MP Master will work right out of the gate for your machine with no changes. You just use the misc integer for the high speed calls. I had Jeremy at DBS Solutions edit mine to get the G05P2 calls working correctly, but I think some of the guys here from the board got it going right in the latest version. G61.1 never has to be cancelled, so you can just put G61.1 wherever you want, and it'll stay active until you hit reset or M30. G05P2 is a PITA to add manually though. It will alarm on any comments or spindle speed changes, so it has to be cancelled (G05P0) and then re-called at the end of every toolpath - so it's important to have the post spit it out correctly.

[TREV]

joe,

thanks for your input. esspecialy in regards to the maxacc2d and mazacc3d

all I was told is we will have a " highspeed option" from the boys in the office.

I sure hope we got more than the g61.1, or some one is going to be unhappy upfront

if they find out they did not ask all the right questions when they bought this.

 

I guesss ill find out for sure Monday when they come to finish the set up of the machine.

 

trevor

[Joe788]

What kind of other machines do you have in the shop right now? What model Fanuc controls are on them?

 

If they're not finished setting up the machine yet - you can save some money by getting those options right away. Otherwise you'll have to pay for somebody to come put in MAZACC3D.

 

When you go in on Monday morning, you can look at the options on the control by hitting the left arrow soft key once or twice until you see the DIAGNOS button, then hit: DIAGNOS>VERSION>OPTION.

 

Options in black are the ones you have, options in white are the ones you don't have. "Shape Comp" is G61.1, "High Speed" is G05P2

 

[TREV]

joe,

 

the fanuc controls are pro 3 and pro a controls all on makino mills 3 vertical and 1 horizontal.

 

the machine just got power to it yesterday and the control has not even been turned on yet

the mill still needs everything set up from bottom up still. the tech guy will be here in the am

to start he is probably going to be here for 2 days to set up and get me started for right now.

I will talk with him and the folks in the office to see what options we actually got. the only obvious

ones to me right now are laser and probe. I need to see control or p.o. to know what else.

thanks

[Zoffen]

Joe pretty much hit it all on the head!

 

All we use is mazak at our shop so i really got used to the no G43 and really like it.

 

To each their own!

[djstedman]

We have a bunch of Mazak's and true they don't need G43 .. that said.. not putting it in is training your guys how to destroy things if they ever get on a Fanuc.. just my opinion but I haven't removed it from our posts.. it doesn't hurt anything having it there and if guys get used to not using it.. they type something into a Fanuc and BOOM.. not good ..

 

As everyone else said.. pretty much the only other things you might want to tweak on the post for that machine is putting in the G61.1 stuff for highspeed machining.. and actually its mostly done if you use the MPMaster control off this site.

[Bennido]

Here in germany there is a company that specializes in MazaCAM, more information you can get here. As far as I know they have a thorough knowledge and also provide english support.