[cncClintain]

Can someone give me the run down on setting tool and work offsets for mastercam programs on mazak mills? We just got mastercam last week and I can't get my tool length offsets or my WPC for my Z right. All of my mastercam experience has been on Haas machines. Its been a year since I've done a setup but before on the Haas I would set the tools off a 1-2-3 block on the table and use a Z offset for my Z zero. I don't like setting tools to the top of the workpiece because if I machine a surface on the part I no longer have my reference to reset tools. If anyone could give me their step by step process it would be greatly appreciated.

[cncnitro]

CncClintain,

On M32, AJV60/120

First thing you need to do is find out if the machine is reading
tool data register for EIA programs, or tool offset register.
You need to read tool data register.

Parameter: F92 bit7- 0=tool offset 1=tool data valid
Change to 1 if 0.
Machine now should be reading tool data page.
Use tool length measuring probe or set tools off table with 123 block.
Enter data in tool data.

Can use WPC or fixture offset (G54-G59)
You can run a Mazatrol program and call out an EIA program with
a Mazatrol sub program call out, or just straight up EIA.

Sample Prog.
(ENTRANCE)

%
O0001
(PROGRAM NAME - SEAL KEEPER 2A )
(DATE=DD-MM-YY - 02-08-11 TIME=HH:MM - 10:51 )
G21
G0 G17 G40 G95 G80 G90
T18 M6 T00
G0 G90 X17.499 Y-20.516 S3150 M3
G43 Z30.
Z4.401 M8
G1 Z-.599 F.25
X-17.922 Y-20.511
G2 X-38.014 Y0. I.423 J20.511
X-17.499 Y20.516 I20.515 J0.
G1 X8.476 Y20.512
/.........
/........
/......
/........
(EXIT)
X17.499 Y-20.926 I-20.925 J0.
G1 X-12.026 Y-20.922
X-17.93 Y-20.921
G2 X-38.424 Y0. I.431 J20.921
X-17.499 Y20.926 I20.925 J0.
G0 Z.349
Z30.
M5
M9
G91 G28 Z0.
G28 X0. Y0.
M30
%

Notice that there's no G49's.
REMOVE ALL G49 CODES!!!! Or Crash is Imminent!!!!!!!!!


G95 is synchronous feed rate. (feed per revolution not inch/min,mm/min)
Like in Mazatrol program feed rates.

No "H" is needed.

Good Luck!

[psychomill]

if you wanted to... you can set up the Mazak the same way you did your Haas using a 1-2-3 block..... there's no difference. Tool Data or Offset works with this. What matters is which side your machine is set to reading for where to put your tool offset...