EIA Issue with M plus Mazak

Was hoping someone might be able to help me out on figuring out the secret sauce to getting a EIA program running on my Mplus control.

I generated a 3D toolpath with Mastercam and posted the code, which it excepted in toolpath verification, but for whatever reason, it seems to continue to want to change tools, even though the specified tool is already in the spindle.

As I understand it, you have to write a tool change code as follows:

T19 T00 M6;

All of the examples in my manual show this format, though this is the first controller that I've had to add the "T00" to in order for it to function. When I didn't have "T00" in the line, it ran on toolpath verification, but alarmed out when I started to actually run the machine.

I suspect I'm having a parameter setting issue that is causing this, but it's uncharted waters for me at this point.

I bought this machine used and it had been years since I ran a Mazak and when I did, I only used Mazatrol. Now I've got some complex parts to run and I'm having a heck of time getting it up to speed with G-code.

Best as I can tell, my parameters are set to read all the tool offsets from Mazatrol, and from what I understand, you can do that even though you're running EIA programs?? The trick at this point is knowing where these parameters need to be set to get this thing fully functional with EIA and Mazatrol.

Any help would be greatly appreciated, as I'm pretty much at my wit's end at this point.

Thanks in advance for any help you can provide.

On my M32 mill, the T19 T00 is setup with no space-

T19T00 M6
G0G90G43H19X0Y0Z6.
Z.1M8

etc.

The T00 is where you might write T19T20M6 to change to T19 and prestage T20 while 19 is doing its thing.

At least that's how I think it works. I run Mazatrol 99.999% of the time.

I have a VTC16B with an umbrella-style changer, so I can't preload tools like you would for a swingarm-style sidemount.

I'm pretty sure the problem lies in the parameters, but I'll eliminate the spacing and see what happens.
It seems like it likes the T019T00M06; since that's what it spits out in MDI mode on a soft key auto tool change.

Matt@Grizzly said:

I have a VTC16B with an umbrella-style changer, so I can't preload tools like you would for a swingarm-style sidemount.

I'm pretty sure the problem lies in the parameters, but I'll eliminate the spacing and see what happens.
It seems like it likes the T019T00M06; since that's what it spits out in MDI mode on a soft key auto tool change.

Click to expand...

Sounds like you're on the right track. . .

Now it will allow me to run, but only after it changes the tool to tool 0. It will ignore it, so long as it believes that Tool 0 is in the spindle.
Tried flipping the T019 and T00 around and it made no difference, but it will alarm out if M06 is in a separate line.
Now I'm trying to restart the dang thing at the G54 line and can't seem to keep from getting a 240 alarm that says it's missing info on an EIA restart.

Frustrating to say the least.

Thought I'd follow up with what I figured out.
From some previous threads I noticed that I need a couple of parameter changes in order for the control to utilize the Mazatrol tool data for offsets in Z. Got that figured and fixed.
Next, I had to include the G43 line in along with the appropriate H# in order for it to recognize the G54 setting from tool to tool.
The book kept saying that if the tool was already in the spindle that it would ignore it and move on in automatic mode. Well, that's true, except for having your single block activated, at which time it pukes and removes the tool from the spindle and replaces it with T00. Provides great tool life, but not many chips..
So, the bottom line is that it needs to have a line is as follows:
T10 T00 M06;
Also, remove G49's as the book says that you're better off to use H00 instead. I never tested it, but since I had it working, why take the chance?

I downloaded a DNC program called DNC Precision, which was recommended sometime back on this site and it works good, all except if you leave it running for long enough for your computer to go into a screensaver or sleep mode, at which time it shuts your computer down. It also likes to hide itself after being minimized, making you think you closed it after the last time you used it. I guess that's the handy feature that you get with the free download model.
Would like to know if there's a reliable one out there that communicates well with a RS232 to USB Null Model Cable that would allow me to send and receive more than 17kb before it gives me the notice that it's time to pay up for rights to own this crasher for a mere $140.00.
I'll make a separate thread in the next day or so outlining the specific parameter settings and communication settings I made to get this thing rolling. With any luck, some other poor fella won't go through what I have in the last several days.

Have 3 different types of long bed mazaks vmc 6 total
Some of them like
T6m6
on same line

Some like
T6
M6
on different lines?

If you get them mixed up they do strange things with tool changes.
one example is
They will tool change and put what ever tool is in waiting in to spindle even if it is wrong tool number??
It will run thinking it has correct tool until it crashes!!

On my VTC 16A only run EIA with auto tool setter I don't have to use M06 at all same goes for H...

N104G91G30X0.Y0.Z0.
N106T05
N108G0G90G54X0.0Y0.0S1200M3
N110G43Z1.M08

You are right there is a setting in parameters that makes it read Mazatrol tool data and not EIA tool offsets
I will look it up when i get to work in the morning.

Adam

OK here we go



F92 bit7 = "1" turns on TOOL DATA page length offset data.
F93 bit3 = "1" turns on TOOL DATA page diameter offset data
F94 bit7 = "0" turns off EIA tool life managment

This way everything is taken care by Mazatrol TOOL DATA page.


Dont forget to power off your control after changes.

Sample program with Mastercam 8




TOOL DATA page M-Plus



EIA tool data page is not used at all.

Kaszub said:

OK here we go



F92 bit7 = "1" turns on TOOL DATA page length offset data.
F93 bit3 = "1" turns on TOOL DATA page diameter offset data
F94 bit7 = "0" turns off EIA tool life managment

This way everything is taken care by Mazatrol TOOL DATA page.
View attachment 133301

Dont forget to power off your control after changes.

Sample program with Mastercam 8

View attachment 133302


TOOL DATA page M-Plus

View attachment 133303

EIA tool data page is not used at all.

View attachment 133304

Click to expand...

Hello,
I hope you can help me, I lost the parameters for a VTC16A with MPlus control. The card got busted so the eeprom parameter backup isno good.
Either way share or sell, your call.

Thank you. My email address is [email protected]

jolulank