Results 1 to 10 of 10

Thread: Mastercam posts on Mazak

  1. #1
    Registered
    Join Date
    Nov 2009
    Location
    United States
    Posts
    75
    Downloads
    0
    Uploads
    0

    Mastercam posts on Mazak

    I am having problems getting the EIA program I created to read the Matatrol tool data page. Problems are occuring in both length and Diameter comps. The tools do not cut at same height as programmed. This could also be due to the use of both having a probe and automatic tool height measurement system both, of which, are broken. Lastly teaching the Z axis coordinate on the EIA side using G54 does not match what I get on a mazatrol work coordinate unit.

    Any help would be great. Hopefully I can return the favor to someone.


  2. #2
    mbi
    mbi is offline
    Registered
    Join Date
    Apr 2008
    Location
    usa
    Posts
    35
    Downloads
    0
    Uploads
    0

    tool length

    First what control do you have?
    I use Eia on our m-32. First you must decide if you are going to program from the center of the cutter or the peripheral of the cutter. I use the center of the cutter and use cutter comp.
    You must set your parameters to read cutter comp. I am at home until Monday and don't have the info handy however it is in your E95 parameter I think?
    Your Mazak will read your tool data page for tool length I think. Check your book to be sure. All our Mazaks use Mazatrol tool Data for tool length.
    You must set all your tool offsets to 0 to control your cutter comp.
    For example:
    Tool # 1 is a 1.0 diameter end mill that is reground to .990. You will put your end mill into pocket #1 and go to you tool offset page and set tool offset comp #1 to -.005.
    Use a D code next to your g41 or g42.
    Teach your WPC’S to G54 and use g54 in your Eia code.
    we also use a probe however you must use the inspection plus software to teach you g54.

    I can't answer why teaching the Z axis coordinate on the EIA side using G54 does not match what I get on a mazatrol work coordinate unit. Our newer m32's to present mazaks you can run a probing unit in your mazatrol program using g54 in your additional wpc's on your wpc line.


  3. #3
    Registered
    Join Date
    Nov 2009
    Location
    United States
    Posts
    75
    Downloads
    0
    Uploads
    0
    The control in particular is a nexus 640. Thank you for the help on the cutter comp. for G41, that makes sense. the parameter settings were already altered and your parameter number is close to the one I had to change. I guess I was hoping that the G41 and G43 commands would match the mazatrol tool offset page in it's entirety.

    For G43, I would use a H# according to the tool I want in the mazatrol tool data page?

    For G41 I would enter a D# in the tool offset page(the one different than the main mazatrol tool offset page) and use the difference in the cutter diameter as the inputted value. Do I have this correct?

    What, exactly, is the inspection plus software and it's capabilities? I will try to look it up online as well.

    Right now both the automatic height measuring system and the probe are broken. In order to complete the part I made I needed to teach each tool off of the workpiece. Can I teach each tool of of a 3" block and back-figure a Z coordinate in order to eliminate teaching every tool off the work?

    Thank you very much for your input.


  4. #4
    mbi
    mbi is offline
    Registered
    Join Date
    Apr 2008
    Location
    usa
    Posts
    35
    Downloads
    0
    Uploads
    0
    You do not need an H with your g43. All you need is g43 and tool number. No H code. It should read the tool data page tool length. There is a parameter for this.

    You are correct on the D code and g41. However check the parameter in your book so your machine knows to read the tool offset page not the tool data page for your tool offsets.

    The inspection plus software is used to probe a plate in g code using macros.


  • #5
    Registered
    Join Date
    Nov 2009
    Location
    United States
    Posts
    75
    Downloads
    0
    Uploads
    0
    Just to double check, the height offset line would look like

    G43 T1

    if using tool 1?


  • #6
    Registered
    Join Date
    Mar 2005
    Location
    Silicon Valley, CA
    Posts
    988
    Downloads
    0
    Uploads
    0
    No.. You do a tool call as normal then for a G43 line, you don't need to specify an H number...

    T1M6
    .
    .
    G43Z.1 (no H)


    This is provided that your parameters and/or Tool Data page isn't telling the machine to look at the Offset page. If you're using the Offset page by iteself, then you need to use H as normal...

    G43H1Z.1
    It's just a part..... cutter still goes round and round....


  • #7
    mbi
    mbi is offline
    Registered
    Join Date
    Apr 2008
    Location
    usa
    Posts
    35
    Downloads
    0
    Uploads
    0

    Sample code of tool length and cutter comp

    This is a sample of the g43 and mazatrol tool data.

    As psychomill said G43 Z 2.0 (no H)



    O2552
    (/////////////////////////////////)

    (Job 2554 2 plate + setup 11-09-2009)

    (\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\)

    (Plate Size 4_STEEL )
    (X 35.5 )
    (Y 17.875 )
    (Z 3 )


    (********************************)
    (WPC X = -28.209 )
    (WPC Y = -25.0975 )
    (WPC Z = -33.567 )
    (********************************)

    ( T97 = EM.75 C CARBIDE )
    N10 G0 G40 G64 G80 G94
    N12 G30 G91 Z0.
    N14 G30 Y0.
    N16 T97
    N18 M6
    N20 G0 G17 G54 G90 X-5.0145Y-9.5171 M38 S 750 M3
    N22 ( T97 DIA.=0.75 NAME=EM.75 C CARBIDE )
    N24 ( FINISH SIDE MILL_WIRE_SLOT_2_150_DEEP )
    N26 M1
    N28 M8
    N30 G43 Z2.0 T97
    Z-1.55
    G1 Z-2.158 F150.0
    G41 D97G62 X-4.8593 Y-8.9375 F10.0
    Y-5.7814
    G3 X-4.9343 Y-5.7064 I-0.075 J0. F7.0
    G1 X-5.0343 F10.0
    G3 X-5.1093 Y-5.7814 I0. J-0.075 F7.0
    G1 Y-8.9375 F10.0
    G40
    X-4.954 Y-9.5171
    X-5.0145
    G41 D97G62 X-4.8593 Y-8.9375
    Y-5.7814
    G3 X-4.9343 Y-5.7064 I-0.075 J0. F7.0
    G1 X-5.0343 F10.0
    G3 X-5.1093 Y-5.7814 I0. J-0.075 F7.0
    G1 Y-8.9375 F10.0
    G40
    X-4.954 Y-9.5171
    G0 Z2.0
    N72 ( PROGRAM END )
    N74 M9
    N76 G0 G28 G91 Z0 M5
    N78 G28 G91 Y0
    N80 G0 G90 G53 X-10.0
    N82 G90 M30


  • #8
    mbi
    mbi is offline
    Registered
    Join Date
    Apr 2008
    Location
    usa
    Posts
    35
    Downloads
    0
    Uploads
    0

    Matatrol tool data page

    Did you change par F93 bit 4? It should look like this 00101000. This Par enables the EIA to read the Matatrol tool data page tool length.

    Just another thought? Is your post outputting code from the tool center or the peripheral? You will need it to output from the tool center. In my cam software I can program from either.


  • #9
    Registered
    Join Date
    Nov 2009
    Location
    United States
    Posts
    75
    Downloads
    0
    Uploads
    0
    I changed that parameter, as well as another one that deals with tool height.

    How does your software differentiate between the tool center or peripheral?


  • #10
    mbi
    mbi is offline
    Registered
    Join Date
    Apr 2008
    Location
    usa
    Posts
    35
    Downloads
    0
    Uploads
    0
    It is just a flag I check if I want to part line program or tool center line program.


  • Similar Threads

    1. MasterCam 5 axis Posts (not free)
      By MrMagooo in forum Post Processors for MC
      Replies: 8
      Last Post: 11-13-2009, 04:52 PM
    2. Editing MasterCam Posts
      By MetalMolder in forum Post Processor Files
      Replies: 8
      Last Post: 10-31-2009, 02:28 AM
    3. Mastercam X2 Posts
      By nerfman in forum Post Processors for MC
      Replies: 11
      Last Post: 07-09-2008, 10:47 PM
    4. Mastercam Posts. How are they supposed to work?
      By Zak@CWS in forum Mastercam
      Replies: 13
      Last Post: 05-03-2008, 11:32 AM
    5. BobCAD posts vs. Mastercam posts
      By justCNCit in forum BobCad-Cam
      Replies: 124
      Last Post: 08-16-2006, 03:17 PM

    Posting Permissions



    About CNCzone.com

      We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

    Follow us on

    Facebook Dribbble RSS Feed


    Search Engine Friendly URLs by vBSEO ©2011, Crawlability, Inc.