Page 1 of 2 12 LastLast
Results 1 to 12 of 13

Thread: fanuc OT

  1. #1
    Registered
    Join Date
    Mar 2005
    Location
    UK
    Posts
    23
    Downloads
    0
    Uploads
    0

    Default fanuc OT

    Hi all,

    I have just bought a Nakamura tome tmc 20 lathe.
    Has anyone got an NC printout they can send me. I need to creat a post for our cam system. I can get the thing to rough and finish but screw cutting seems a problem. The tool just overides in X every time and I can't understand why.

    Cheers,
    Paul.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Dec 2006
    Location
    usa
    Posts
    247
    Downloads
    0
    Uploads
    0

    Default

    What treading cycle are you using. I know g76 has a parameter that sets cut depth. mine was set at .0001 so the first time I threaded with it it took about 20 minutes. I believe if you use p1 it uses your d amount for depth of cut, I don't remember for sure so I use g92 instead. My controller is 11te so it doesn't use the double line cycles.
    Joe



  3. #3
    Registered Sump Cleaner's Avatar
    Join Date
    Dec 2005
    Location
    Canada
    Posts
    55
    Downloads
    0
    Uploads
    0

    Default

    Paul,

    Here is a snippit from our TMC 15 with an explanation

    %
    M1(THREAD 1 3/16-20)
    G20G40G80G97G99
    T0404(SER 0750 K16)
    (INSERT - 16ER-20 UN)
    G0X1.2S2500M3
    Z.15M8
    G76P000060Q150R10
    G76X-1.114Z-.37R0P320Q140F.05
    G0Z1.M9
    G28W0M5
    M30
    %

    G76 P(m)(r)(a) Q(min) R(fin)
    G76 X(fin) Z(len) R(i) P(k) Q(1st) F(L)

    WHERE
    m = SPRING CUTS (01)
    r = CHAMFER AMOUNT(00)
    a = TOOL ANGLE (80 60 55 30 29 0)
    min = MINIMUM DEPTH OF CUT
    fin = FINISHING ALLOWANCE
    fin = ROOT DIAMETER
    len = LENGTH OF THREAD
    i = THREAD RADIUS DIFFERENCE
    k = THREAD HEIGHT (RADIUS)
    1st = 1ST CUT DEPTH
    L = THREAD LEAD

    Hope this helps...

    JK



  4. #4
    Registered
    Join Date
    Mar 2005
    Location
    UK
    Posts
    23
    Downloads
    0
    Uploads
    0

    Default

    Hi JK,

    Thanks for taking the time to send that to me. I can work with this.

    Thanks again,

    Paul.



  5. #5
    Registered
    Join Date
    May 2006
    Location
    Sweden
    Posts
    265
    Downloads
    0
    Uploads
    0

    Default

    Does oT use the 2 line G76 cycle?



  6. #6
    Registered
    Join Date
    Mar 2005
    Location
    UK
    Posts
    23
    Downloads
    0
    Uploads
    0

    Default

    yes it does...



  7. #7
    Registered
    Join Date
    May 2006
    Location
    Sweden
    Posts
    265
    Downloads
    0
    Uploads
    0

    Default

    Wich fanuc uses the one liner cycle?



  8. #8
    Registered
    Join Date
    Dec 2006
    Location
    usa
    Posts
    247
    Downloads
    0
    Uploads
    0

    Default

    I know 11 uses 1 line.



  9. #9
    Registered dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2674
    Downloads
    0
    Uploads
    0

    Default

    I believe the 0, 16, 18, & 21t controls may be able to use the 1-line Multiple Repetitive Cycles (G71-G76). Check your settings for "TAPE-F". If 0, it uses 2-line cycles, if 1 it uses 1-line cycles. Check your operator's manual under "Memory Option Using Series 10/11 Tape Format". Be aware that this also changes sub-program call loop format to M90 Pnnnn Lnnnn.



  10. #10
    Registered
    Join Date
    Mar 2005
    Location
    UK
    Posts
    23
    Downloads
    0
    Uploads
    0

    Default error alarm

    I can now run my program through all the operations without any errors. However when I cycle the program again, it alarms out when it reads the first moves within the roughing cycle. The error is listed as 'feedrate not commanded or feedrate inadequate'. If I restart the machine it runs ok for the first time then errors out if I try to cycle it again.
    I take this to mean the program is setting up something later in the program which, when read again, creates a fault but I can't think what it could be.
    Any ideas?



  11. #11
    Registered dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2674
    Downloads
    0
    Uploads
    0

    Default

    It would help if we could see your code, but...

    1. Make sure there's a feedrate commanded in or before your first feed move.

    2. Make sure that G99 (IPR) is active. If you're using G98 to pull stock, etc. you'll get that alarm if you have a small F value.



  12. #12
    Registered
    Join Date
    Mar 2005
    Location
    UK
    Posts
    23
    Downloads
    0
    Uploads
    0

    Default More trouble

    Hi, and thankyou decoupar for the G99 advice. It worked. Great.

    Does anyone know a drill cycle that retracts in Z to an absolute figure, say 3mm. At the moment it retracts by an incremental amount.

    Last edited by Paul Goddard; 05-24-2007 at 11:59 AM.


Page 1 of 2 12 LastLast

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 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