584,874 active members*
5,100 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Mastercam > Adding Custom Drill Cycle to MCX6
Results 1 to 9 of 9
  1. #1
    Join Date
    May 2004
    Posts
    4519

    Adding Custom Drill Cycle to MCX6

    I am wanting to add a custom drill cycle to MCX6 to use a deburr tool (this one - Power Deburring Tools | MSCDirect.com) at the top and bottom of the hole. The pilot length is 0.680". The length from the tip to the back of the blade is 1.000". The code to run the tool looks basically like:

    G01 Z-0.68 F10.
    G04 P0500
    G01 Z-1.125
    G01 Z-1.
    G04 P0500

    I have edited the post processor at the Post Text for:
    [CTRL_MILL|GENERIC HAAS 3X MILL TEST]

    [drill cycle 9]
    1. "Deburr - Special Cycle"
    7. ""
    8. ""
    9. ""
    10. ""
    11. ""
    [drill cycle descriptions]
    9. "Deburr - Special Cycle"

    So, now it shows up in my cut parameters as a cycle (see attachment). What I can't figure out is how to define the custom drill parameters in the post processor. Then I know I need to figure out how to apply those parameters in the post processor to output the code desired.

    Kind of busy with other things at the moment. No idea when I might can get back to this.
    Attached Thumbnails Attached Thumbnails DRILL CYCLE 1.jpg  

  2. #2
    Join Date
    May 2004
    Posts
    4519
    I found in the NCI file where it outputs the data for the custom drill parameters:

    20700
    0 0 0 0 0 0 0 0 0 0
    1001
    0 100 10 90 90 90 0 7601 72.979104 0 0. 0. 0.1 10. 10. 10. 0 0.
    0
    0 0. 0. 0.1 -2. 0
    82
    1. 2. 3. 4. 5. 0. 0. 0. 0. 0. <<<<<custom drill parameters #1 - #10
    81
    8 0. 0. -0.41 0.5 72.979104 0.1 0.1 0.1 0.1 0.1 0.1 0. 0.1 0. 0. 0.1 3000 0 0.
    80

  3. #3
    Join Date
    Aug 2008
    Posts
    90
    Do you have the MP Post Reference guide? If you do not, I would suggest getting it.

    The information in the guide will help you to get what you are looking for.
    Attached Thumbnails Attached Thumbnails 2013-01-09 06_48_58-106 Post TXT File.png   2013-01-09 06_53_13-106 Post TXT File.png  

  4. #4
    Join Date
    May 2004
    Posts
    4519
    Thanks. I am sure that information will lead to more questions. But it is a good start. Maybe I can work on it some more in the next couple of days.

  5. #5
    Join Date
    Aug 2008
    Posts
    90
    If you look through the existing drill cycles you can match them up with the pages from the document. That will help you understand what is going on and what is needed.

    I think that you can get the post reference guide from your reseller. They give them away for free. It is from V9 but any changes that have been made or added are in the documentation with the current version of Mastercam.

  6. #6
    Join Date
    May 2004
    Posts
    4519
    Got the custom cycle added into the post text section and it shows up in the drilling operations now under [drill cycle 9].

    # --------------------------------------------------------------------------
    # POST TEXT
    # --------------------------------------------------------------------------
    [CTRL_MILL|GENERIC HAAS 3X MILL TEST]
    [misc integers]
    1. "Work Coordinates [0-1=G92, 2=G54's]"//2
    2. "Absolute/Incremental, top level [0=ABS, 1=INC]"
    3. "Reference Return [0=G28, 1=G30]"
    [simple drill]
    1. "Drill/Counterbore"
    7. ""
    8. ""
    9. ""
    10. ""
    11. ""
    [peck drill]
    3. ""
    7. "Peck"
    8. ""
    9. ""
    10. ""
    11. ""
    [chip break]
    3. ""
    7. "Peck"
    8. ""
    9. ""
    10. ""
    11. ""
    [tap]
    3. ""
    7. ""
    8. ""
    9. ""
    10. ""
    11. ""
    [bore1]
    1. "Bore #1 (feed-out)"
    7. ""
    8. ""
    9. ""
    10. ""
    11. ""
    [bore2]
    1. "Bore #2 (stop spindle, rapid out)"
    3. ""
    7. ""
    8. ""
    9. ""
    10. ""
    11. ""
    [misc1]
    1. "Fine Bore (shift)"
    7. ""
    8. ""
    9. ""
    10. ""
    [misc2]
    1. "Rigid Tapping Cycle"
    3. ""
    7. ""
    8. ""
    9. ""
    10. ""
    11. ""
    [drill cycle 9]
    1. "Deburr - Special Cycle"
    2. ""
    3. "Dwell"
    4. ""
    5. ""
    6. "Chamfer depth"
    7. "Pilot length"
    8. "Back blade length"
    9. "Part thickness"
    10. "Clearance"
    11. ""
    [drill cycle descriptions]
    1. ""
    2. ""
    3. ""
    4. ""
    5. ""
    6. ""
    7. "Fine bore (shift)"
    8. "Rigid Tapping Cycle"
    9. "Deburr - Special Cycle"
    [canned text]
    1. "Stop"
    2. "Ostop"
    3. "Bld on"
    4. "bLd off"
    5. "M5"
    6. "M6"
    7. "M7"
    8. "M8"
    9. "M9"
    10. "M10"
    [CTRL_TEXT_END]

  7. #7
    Join Date
    May 2004
    Posts
    4519
    Now working on how to impliment it to output the code. Any idea what the variable is for "Top of Stock"? I need to use that for a calculation in the post. I know the other variables are:

    initht$ - Clearance
    refht$ - Retract
    pfzout - Depth
    peck1$ - 1st peck
    peck2$ - Subsequent peck
    peckclr$ - Peck clearance
    retr$ - Retract amount
    dwell$ - Dwell
    *feed - Feed

    Besides Top of Stock, what else might I be missing?

  8. #8
    Join Date
    Aug 2008
    Posts
    90
    tosz (tosz$) is the "absolute" position of the Z location of the top of stock

  9. #9
    Join Date
    May 2004
    Posts
    4519
    Thanks. That helps.

Similar Threads

  1. Matsuura MC-500V2 Adding Custom 4th Axis?
    By Techbuilder in forum Uncategorised MetalWorking Machines
    Replies: 2
    Last Post: 07-12-2011, 08:36 AM
  2. Adding cycle start to mach 3 mill
    By Dr Doofensmirtz in forum Mach Mill
    Replies: 4
    Last Post: 03-06-2011, 02:59 AM
  3. Custom Macro for Finding Cycle time
    By yaji63 in forum G-Code Programing
    Replies: 8
    Last Post: 02-08-2011, 04:58 AM
  4. Adding dro to mill/drill machine
    By trailblazer in forum Uncategorised MetalWorking Machines
    Replies: 0
    Last Post: 02-14-2010, 04:51 AM
  5. Adding drill points to a rectangle
    By Joe Rodney in forum Mastercam
    Replies: 6
    Last Post: 10-19-2008, 09:35 PM

Posting Permissions

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