Newbie- Using cutter comp eia/iso on M2

[apylus444]

Hello,
I'm using EIA/ISO/ format on M2 controller. I want to offset (G41) my cutter, when I go to the tool offset page and put -.005 it just goes that much deeper with z axis. I see that one cannot put a negative value in the tool data page. Does anyone know how to offset on the x and y plane? Thanks in advance.

[MrMazak]

Check parameter OP2 and set it for what you need

OP2 bit 0 Tape Puncher (0=EIA 1=ISO)
bit 1 Tool Length Offset (0=Only Z axis 1=Any axis)
bit 2 Tool Offset (0=D code 1=H code)
bit 3 Tool Dia Offset (0= Diameter in TOOL DATA is active 1 = not active)

To use Mazatrol Tool Data in EIA programs set all to 0 and delete any G43 and D or H callouts in your program just use T01 to call tool #1 and it will use the Tool length and Actual Dia. from the TOOL DATA page.

[apylus444]

From what I have found out it may have something to do with a parameter needing to be changed??? Any ideas?

[MrMazak]

Read my previous post and you will have the answer.

[apylus444]

My current setting with op2 is 248. The description is 76543210 with corresponding 1 and 0 values (1 for H, 0 for D, etc). I learned that 7 is 128, 6 is half that (64), 5 half that, etc until 0 = value of 1. I calculate that the setting should be 240, I'll try that. Thanks for the reply Mr Mazak.

[apylus444]

This is a copy of my correspondence with MrMazak on the issue for any who may benefit
apylus444

Re: a previous thread on cutter comp M2

Originally Posted by apylus444 Originally Posted by MrMazak 240 should be right, be sure to delete any G43 D or H codes and start the tool at least 50% of the diameter from were you want comp to start. If you want a sample program let me know. I would love to see a sample. Could you also include instructions on actually offsetting, i.e. do you put dia offset in data page or offset page, etc.? I understand the 50% lead in principle. Much thanks, Apylus444

%
O1
(PGM FOR M-PLUS USING IPR FEED)
(FILE NAME: TEST1.NC)
()
G54G40G80G90M01
N1
(ABOVE SEQ# SHOULD BE 1ST TOOL)
G0G91G28Z0
G90
M06 T1(.75D X 1-5/8 LOC 4 FLUTE CARBIBE)
M01
G17G54G0X-.375Y-.4Z4.M3S2037M8
G95
G41
Z.1
G1Z-.75F.0031
Y0.F.0047
Y6.32
Y6.72
G0Z4.
G40
G41
X10.355
Z.1
G1Z-.75F.0031
Y6.32F.0047
Y0.
Y-.4
G0Z4.
G40
M09
G0G91G28Z0
G90
M06 T2(.5D X 1-5/8 LOC 4 FLUTE CARBIDE)
M01
G17G54G0X-.25Y-.3Z4.M3S9167M8
G95
G41
Z.1
G1Z-.75F.0031
Y0.F.0047
Y6.32
Y6.62
G0Z4.
G40
G41
X10.23
Z.1
G1Z-.75F.0031
Y6.32F.0047
Y0.
Y-.3
G0Z4.
G40
M09M05
G0G91G28Z0
G90
M06 T1
(FIRST TOOL LOADING)
(END OF PROG.)
M30
%[/QUOTE]

Thanks MrMazak. One final question: can you program toolpaths with cadcam for automatic tool compensation; i.e. the center of the cutter (and dia offset would = 0) or do you have to program so that you put the actual dia of the tool in the tool data page? And where do you offset: tool data page or tool offset page?
Thanks for all the help, I'm going to copy this and add it to the thread I started a while ago so that others might benefit.
Apylus444[/QUOTE]

The program I sent uses .750 for the tool diameter with offset of 0.0 I could also program tool diameter of 0.0 and use Mazatrol Tool Data for the comp. (which is what I usaully do)

[compuslave]

I despise mazatrol so I only do eia programming on mine and had issues with cutter comp in the beginning too. For one don't use the tool data meant for mazatrol, goto eia/iso info and choose tool offsets. And I have gotten in the habit of putting a G17 at the begining of my programs to lock it into X-Y plane. Mazak parameters especially on old machine are a confusing mess mostly due to the poorly translated manuals.

Hope this helps.

[MrMazak]

Sounds like you have some anger issues with Mazak compuslave. If you would give mazatrol a chance you probably would abandon that ancient code and be more productive to boot. Many old time "programmers" lost there jobs because of mazatrol and there lies alot of resentment. That said, embrace any technology that can make you more competitive, Mazatrol is one such technology. The way manufacturing is going we all need to use any tool we can to survive.

[compuslave]

Not anger just a preference. I'm a macro fiend and you can't exactly do that in mazatrol, or any conversational control for that matter. Besides, the idea of platform dependence rubs me wrong too which is why I stopped using microsoft products more than ten years ago. I'm not worried about my job or place in the market because I do what I do well. I am a toolmaker first and programmer second. Don't take my comments personal buddy