[ntcnc]

Hello all

I have been a member for many years I can usually search and find what I am looking for but couldn't this time so here is my first post!

I am trying to help out a nearby shop that purchased a Mazak V-20. It is a 1985 vintage with the M-2 control. They bought it to run somewhat complicated casting on it. They have asked me to help program and get them going. I have not been on a Mazak for almost 10 years and would rather program on Mastercam than Mazatrol. I am writing a post for Mastercam and would like a little info from some users. This is what I need. Basically it is so I can get the tool changes right.

How is the tool changes called out? from what I seen in the manuals they gave me Txxx and M06 can not be called in the same block. How do you set up next tool? Can I use G91 G28 Z0. call before the tool change? Do I need to send X and Y too?

This is the way I was setting up but would like to verify before I run on machine

(First tool change)
T10
G91 G28 Z0.
M06
T11 (next tool)

(all other tool changes)
G91 G28 Z0.
M06
T12 (next tool)

Any input would be appreciated.

Thanks

Jerry

[60rock]

Some machines need to load the tool into the "Pod" first. Although I can't be positive I would try calling up the tool first.

T#(should get tool ready in changer)

Then M6 to perform the change.

You should then be able to call up the next tool to be used later in the program.

The G91 G28 Z0 may not be the tool change position either.

[MrMazak]

Below are two examples for M+ or M32, M2 should be similar. First one uses G28 second one uses G30. Sometimes M06 needs to be on the same line others it is on a separate line. Try them until you find one that works. (note: these programs are for using Mazatrol Tool Data for offsets! no G43 D-H is used)



O00000001
G00 G40 G80 G90
N1 M6 T01 (5G ISCAR MILL)
S3056 M03 T02
G00 G54 X5. Y-2.7198 B0.
M08
Z4.
G95
Z.15
G01 Z0. F.06
X-6.22 F.004
G02 Y-2.25 R.2349
G01 X5.
G00 Z4.
M5 M9
G91 G28 Z0
9
N2 M6 T02 (1.66B SAE-12 ALLIED)
M1
S1553 M03 T03
G00 G90 G54 X-1.3 Y-3.3 B0.
M08
Z4.
G95
etc..........OR


(======= START OF PROGRAM =======)
N100 G20
N102 G0 G17 G40 G80 G90 G95
(3/4 BALL ENDMILL TOOL26 DIA .750 )
( FAR SIDE ROUGH .025 STK )
N104 G30 G91 Z0. Y0.
N106 T26
N108 M6
N110 T1
N112 S10000 M3
N111 G61.1
N114 G0 G90 G55 X2.338 Y6.1892
N116 Z2.5 M8
etc

[rusty1979]

on my nexus 410 i program a tool call in iso like this it is safe aswell

N1 G00 G90 M09 (ABOSOLUTE POSITIONING)
G53 Z0 M05 (RETURN TO SAFE MODE)
T1?? (PRE CALL TOOL)
M06 (TOOL CHANGE)
G00 G90 G55 X? Y? M03 S????(POSITION TOOL TO START OP)
G00 Z5? (RAPID TO POSITION REQ)