[maramb]

Machine : Mazak Integrex 200 III St whith 2 spindels, 1 lower turret (for lathe) and 1 upper turret whith a tool magazin 40 pcs

I want to repeat in ISO the code on my Mazak whith a produkt counter, I have tried the DO1 and GOTO options.
The problem is that when I jump up to the beginning of the code,where the counter should be set to +1 one of the turrets doesn't get any code (depending on the G109L1 or G109L2), it's got to do something whith the waiting codes I guess but I can't find what it is.

has any of you had these problems and how did you solve it ?

thnx

[ajl6549]

The parts counter may not work with eia/iso only mazatrol. If you use mazatrol in the " end line " it asks parts count? (y/n)? but eia/iso...?

[ajl6549]

you may be able to use a mazatrol prog as a sub and turn on the counter that way???

[maramb]

I am building a postprocessor for Mastercam and we want to put out a program that is 100% correct, we are going to "disable" the mazatrol controller !

so it should be only ISO code !

[EVERFABCHAD]

Run a Mazatrol sub in your EIA program

[maramb]

Run a Mazatrol sub in your EIA program

that is an option, but I would like to find a way to put in my NC-code without any sub programs

[ajl6549]

I would say to contact your mazak dealer tech support maybe they can help. But i'm fairly shur it's an feature for mazatrol only.

[maramb]

pfffff, typical Mazak to add options in the mazatrol that can't be used in ISO.

I've contacted the tech supplier but it seems to be tough to answer questions for ISO code, they can tell you everything about mazatrol

thanks for your answers, I'm still gonna try to get it to work

[ajl6549]

Try to make a "dummy prog" in mazatrol, just enough lines to let it read. In the end statment say yes to counter. Next, run it w/single blk on and observe buffer or next portion of the display esp. when it reads the "end statment" you may be able to catch a few " oddball M or G codes and one of theses mite make the counter work???, good luck... never mind the above doesn't work. It looks like a mazatrol sub prog might be your only opption. On the plus side I did try the sub. idea on ours (640 m control) and it works fine. If you need help with the Mazatrol sub. write back I can give you an sample.

[maramb]

I'll wait 'till my tech supplier answers me and let you know when I tested the file on the Mazak

thnks for the example option but I still want to solve this in the Post

[CNCRim]

I don't know what you try to do, but I believe that you are program counter in macro I see you used DO and GOTO. I recommend you should use While...DO don't use GOTO. If you have use GOTO statement I believe if you have a long program the machine will give you about 1 second pause because it have to look throught program from head to bottom. For WHILE loop it more efficent.

I don't his the example you look for:
#100=1
While[#100GT180]DO 1
G1 XYZ..
XYZ......
XYZ.....
M253(Part counter if I remember it right)
#100=#100+1
END 1

hopefully It will help you.

[Integrexman]

Here is a new forum just for mazak Integrex machines http://integrexmachinist.com/.

[sakis]

Try M199P(program number)Q1 inplace of the M30. Or try M198P(program number)Q1 inplace of M99.

ex.

%
O1(example)

N100
G28U0
T0101.0
;
;
;
;
etc.
M199P1Q1
%
M199P1Q1 will run the program once and increment the counter and stop.
M198P1Q1 will run the program until the counter is met.

[maramb]

thnx, gonna try the M199/M198 soon :cheers:

and thnx for the link integrexman, see you there

[cnclogistics]

Parts count (#3901, #3902)
Use of variable numbers 3901 and 3902 allows the actual value and the desired value of parts
count to be read or substituted.
Value type Variable number
Actual value 3901
Desired value 3902
- These variables must be integers from 0 to 9999.
- Data reading and writing by these variables is surely suppressed during tool path checking

[maramb]

thnx for the reply, gonna try this on the machine.

do you know if the parameters are resetted when I call a new ISO program ?
the machine does that when the barfeeder (LNS) pulls a new stock, it's a mazatrol program with a subprogram, the sub is my ISO file

[cnclogistics]

thnx for the reply, gonna try this on the machine.

do you know if the parameters are resetted when I call a new ISO program ?
the machine does that when the barfeeder (LNS) pulls a new stock, it's a mazatrol program with a subprogram, the sub is my ISO file

The parameters are not reset. The only time the bar feeder resets is during e-stop or you switch the bar feeder mode switch off.

[out2thow]

just put this in your EIA program to trip the counter

#3901=#3901+1

-S

[andrejl]

hello peoples!
I have problem with changing tools. Mazak h630.
After loading tool, tool shifter go back between parked A and parked B.After this, tool shifter can't be moved in auto mode. I must go to handle mode, and then move tool shifter to parked A or B.
I need some a program with often changing tools.
If can help me, please send me a mail to [email protected]

[andrejl]

hello peoples!
I have problem with changing tools. Mazak h630.
After loading tool, tool shifter go back between parked A and parked B.After this, tool shifter can't be moved in auto mode. I must go to handle mode, and then move tool shifter to parked A or B.
I need some a program with often changing tools.
If can help me, please send me a mail to [email protected]