G76 on Fanuc 15-TF - bizarre operation


Results 1 to 4 of 4

Thread: G76 on Fanuc 15-TF - bizarre operation

  1. #1
    Member
    Join Date
    Jan 2008
    Location
    usa
    Posts
    78
    Downloads
    0
    Uploads
    0

    Default G76 on Fanuc 15-TF - bizarre operation

    I need some help making G76 multi-repeat threading work.
    The machine is a Daewo Puma 8HC-3A with Fanuc 15-TF control.
    I want to thread 1/8” NPT on brass.
    27 Threads Per Inch, thread lead = 0.037037”. Will simplify to .037”
    From charts, thread depth = .027”
    From charts, the thread length is ~3/8, so I will use .4” to be threaded onto my brass
    Major dia at big end from charts is .405
    The tool start will be positioned .2” in front of stock, making that a Z0.200” dimension, a Z total travel of .6”.
    Extending he slope of standard pipe threads makes the X position at that lead-in to be 0.3675”
    Total X diameter change over Z stroke of .600” is: .405 - .3675 = .0375”
    In trying to understand the G76 operation, I want a 1st cut depth of .001”, a minimum cut depth of .001”, finish allowance .001”, and 1 finish pass.

    Here is the code I have tried:

    (THREADING HERE)
    G20 G56 G90
    G97 G98 M17
    M42
    G50 S2000
    T0606
    G00 X1. Z5.0
    M03 S60
    M08
    Z.200
    X.3675
    G76 P010060 Q10 R10
    G76 X.351 Z-0.400 P270 Q10 R-375 F.037
    G00 X8. Z10.0 M05
    M09
    M30
    %

    Removed stock from chuck, so as to just observe process cutting air.
    The above code (with S700 code) results in 10 threading passes, but they didn’t look right.
    Changed to S60 so as to observe what’s going on. I monitored the X & Z positions during the threading passes, and X DID NOT CHANGE during the Z movement from +.2 to -.4
    And the X values didn’t make sense to me. Below is what I observed for X positions during the 10 passes.

    Pass # X @ start X @ end
    1 .361 .361
    2 .371 .371
    3 .381 .381
    4 .391 .391
    5 .401 .401
    6 .411 .411
    7 .421 .421
    8 .276 .276 <<<<<==== ??
    9 .351 .351

    Very bizarre results.

    Sure need some help with this.

    Cheers

    Similar Threads:


  2. #2
    Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1792
    Downloads
    0
    Uploads
    0

    Default Re: G76 on Fanuc 15-TF - bizarre operation

    Quote Originally Posted by serickson View Post
    G76 P010060 Q10 R10
    G76 X.351 Z-0.400 P270 Q10 R-375 F.037
    Many things are parameter dependent. May try the following:
    Replace R10 by R0.001
    The min DOC must be smaller than the first DOC. Therefore, replace Q10 in the second block by Q20
    Replace R-375 by R-0.0375/2 i.e., R-0.01875 (R is a radius value). Use a rounded figure R-0.0188

    Also, delete G90 in the first block. I believe, you are using G-code system A.
    In inch mode, up to six digits after decimal are allowed for F, irrespective of the increment system being used on the machine, though it is IS-B, mostly.
    Therefore, for better accuracy, may use F0.037037

    For detailed information about threading (G92, G76, G32 & G34), may refer to this.

    Last edited by sinha_nsit; 10-17-2018 at 02:07 PM.


  3. #3
    Member
    Join Date
    Jan 2008
    Location
    usa
    Posts
    78
    Downloads
    0
    Uploads
    0

    Default Re: G76 on Fanuc 15-TF - bizarre operation

    Thanks for the response. I will be trying your suggestions tomorrow, but I did come across information in the yellow Fanuc book that has allowed me to successfully make the G76 threading operation work.
    From the book: G76 X__ Z__ I K D F__ A__ P__
    The actual code that worked for me was:


    (G71 MULTI PASS TURNING)
    (MAKE STRAIGHT TAPER)
    ( TO ACCEPT THREADING)
    G00 X.55 Z0.2
    G71 P200 Q201 U0.01 W0.010 F.007 D0150
    N200 G01 X0.380 Z0.0 F.05
    X.405 G01 F.007 Z-.400
    N201 X.55 Z-0.475
    G70 P200 Q201
    G00 X.7
    M05
    M09 G00 X10.0 Z10.

    (NEW G76 TEST)
    G20 G56 G90
    G97 G98 M17
    M42
    G50 S2000
    T0606 S1450
    G00 X.45 Z.2 M08
    M03
    G76 X.351 Z-.4 I-.0187 K.027 D0020 F.037 A60 P1
    M05
    M09
    G00 X8. Z10.
    M30


    Again, Thanks
    Steve



  4. #4
    Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1792
    Downloads
    0
    Uploads
    0

    Default Re: G76 on Fanuc 15-TF - bizarre operation

    This is 1-block format.
    A machine is set for either 1-block or 2-block formats. Both do not work at the same time.



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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

G76 on Fanuc 15-TF - bizarre operation

G76 on Fanuc 15-TF - bizarre operation