535,633 active members*
3,759 visitors online*
Register for free
Login
Results 1 to 12 of 12
  1. #1
    Registered
    Join Date
    Dec 2006
    Posts
    35

    Using cutter comp eia/iso on M2

    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.

  2. #2
    Registered
    Join Date
    Dec 2007
    Posts
    300
    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.

  3. #3
    Registered
    Join Date
    Dec 2006
    Posts
    35
    From what I have found out it may have something to do with a parameter needing to be changed??? Any ideas?

  4. #4
    Registered
    Join Date
    Dec 2007
    Posts
    300
    Read my previous post and you will have the answer.

  5. #5
    Registered
    Join Date
    Dec 2006
    Posts
    35
    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.

  6. #6
    Registered
    Join Date
    Dec 2006
    Posts
    35
    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
    Quote Originally Posted by apylus444
    Quote 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)

  7. #7
    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.

  8. #8
    Registered
    Join Date
    Dec 2007
    Posts
    300
    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.

  9. #9
    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

  10. #10
    Benutzer
    Join Date
    Jan 2010
    Posts
    107

    Re: Using cutter comp eia/iso on M2

    Hello

    I have changed the parameters but i still dont get the tool offset lenght correct.. my tools go below the Z surface..


    O1001
    (T4 D=10. CR=0. - ZMIN=-1. - FLAT END MILL)
    N10 G90 G94 G17 G49
    N15 G21
    N20 G53 G0 Z0.

    (BORE1)
    N25 T4 M6
    N30 S6000 M3
    N35 G54
    N40 M8
    N45 G0 X32.678 Y-119.177
    N50 Z100.
    N55 G0 Z22.
    N60 G1 Z20. F500.
    N65 G41 X31.778 Y-113.177
    N70 G3 X25.778 Y-119.177 I0. J-6.
    N75 X39.578 Z19. I6.9 J0.
    N80 X25.778 Z18. I-6.9 J0.
    N85 X39.578 Z17. I6.9 J0.
    N90 X25.778 Z16. I-6.9 J0.
    N95 X39.578 Z15. I6.9 J0.
    N100 X25.778 Z14. I-6.9 J0.
    N105 X39.578 Z13. I6.9 J0.
    N110 X25.778 Z12. I-6.9 J0.
    N115 X39.578 Z11. I6.9 J0.
    N120 X25.778 Z10. I-6.9 J0.
    N125 X39.578 Z9. I6.9 J0.
    N130 X25.778 Z8. I-6.9 J0.
    N135 X39.578 Z7. I6.9 J0.
    N140 X25.778 Z6. I-6.9 J0.
    N145 X39.578 Z5. I6.9 J0.
    N150 X25.778 Z4. I-6.9 J0.
    N155 X39.578 Z3. I6.9 J0.
    N160 X25.778 Z2. I-6.9 J0.
    N165 X39.578 Z1. I6.9 J0.
    N170 X25.778 Z0. I-6.9 J0.
    N175 X39.578 Z-1. I6.9 J0.
    N180 X25.778 I-6.9 J0.
    N185 X39.578 I6.9 J0.
    N190 X33.578 Y-113.177 I-6. J0.
    N195 G1 G40 X32.678 Y-119.177
    N200 G0 Z50.
    N205 X33.178 Y-118.177
    N210 Z1.
    N215 G1 Z0. F500.
    N220 G18 G3 X32.178 Z-1. I-1. K0.
    N225 G17
    N230 G1 G41 X31.678 Y-113.177
    N235 G3 X25.678 Y-119.177 I0. J-6.
    N240 X39.678 I7. J0.
    N245 X25.678 I-7. J0.
    N250 X31.678 Y-125.177 I6. J0.
    N255 G1 G40 X32.178 Y-120.177
    N260 G18 G2 X33.178 Z0. I0. K1.
    N265 G0 Z100.
    N270 G17

    N275 M5
    N280 M9
    N285 G53 G0 Z0.
    N290 M30

  11. #11
    Benutzer
    Join Date
    Jan 2010
    Posts
    107

    Re: Using cutter comp eia/iso on M2

    ok so i got it to read diameter offset. but not lenght... i still need to put tool lenght into the EIA offset page.

  12. #12
    Registered
    Join Date
    Aug 2005
    Posts
    116

    Re: Using cutter comp eia/iso on M2

    Quote Originally Posted by MrMazak View Post
    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.
    Mr. Mazak,

    Hi. I did what you said and OP2 for me is 224 right now. Deleted all the G43 H and G42 D codes (a hard thing for a G-code guy to do!) and yes the machine magically uses the Mazatrol tool length.

    I must be violating another fundamental rule though, as I try to take a .125 endmill in to open up a .178 semi-finished (without comp) milled hole to .188. I get "512-Tool Diameter Offset Impossible". I would think it IS possible to get tool comp working in such small hole.

    Thanks for your reply!

Similar Threads

  1. Cutter Comp?
    By starvinmarvin in forum MadCAM
    Replies: 16
    Last Post: 09-28-2013, 11:05 PM
  2. M2 cutter comp help
    By nlh in forum Mazak, Mitsubishi, Mazatrol
    Replies: 2
    Last Post: 06-02-2009, 05:59 PM
  3. Cutter Comp.
    By Bob Z1 in forum Uncategorised CAM Discussion
    Replies: 2
    Last Post: 05-28-2009, 04:21 PM
  4. Cutter comp on an id hole< cutter diam.??
    By PaintItBlue in forum Haas Mills
    Replies: 5
    Last Post: 05-06-2008, 12:30 AM
  5. Cutter Comp?
    By donl517 in forum Fadal
    Replies: 5
    Last Post: 07-03-2007, 02:36 PM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •