Results 1 to 9 of 9

Thread: g76 threading cycle (2 block g76)

  1. #1
    Join Date
    Jul 2010
    Posts
    5
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default g76 threading cycle (2 block g76)

    how do u change infeed to alternating? we have a new part that we have to thread on a fanuc 18t control. or just a compound infeed is it the first line p011060 or is it some paramiter . any help would be apreciated
    the rookie threader

  2. #2
    Join Date
    Jul 2009
    Location
    Columbus, ohio
    Posts
    246
    Thanks
    0
    Thanked 19 Times in 18 Posts

    Default Re: g76 threading cycle (2 block g76)

    What do you mean by alternate threading?
    Do you want the infeed to alternate from front to back?
    Some of the older, and way more expensive controls had this option, but I think you need to stick with the angle input that corrects the infeed for the angle you are calling out in the first line of the G76 as it goes deeper.
    If you have other questions, look at the examples I have on my website.
    www.doccnc.com
    Heinz.

  3. #3
    Join Date
    Jul 2009
    Posts
    96
    Thanks
    0
    Thanked 10 Times in 10 Posts

    Default Re: g76 threading cycle (2 block g76)

    To do alternate flank infeed in the G76 cycle on a 0i , 18i ,21i control you have to use the old one line cycle format.

    Example:

    G76 X2.29 Z-1.0 K1560 D500 F.25 A60.P2

    The P2 is the code that switcheds on alternate flank infeed.

    K- Thread depth per side.
    D- Depth of first cut
    A- Included angle

    Please let us know how it goes.

    Regards
    Deon

  4. #4
    Join Date
    Nov 2006
    Posts
    40
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: g76 threading cycle (2 block g76)

    Are you sure you wouldn't have to set a parameter to be able to switch to the single-line G76 format?

    My Fanuc book for the 18T control shows parameters in a range of 5130-5132 and 5140-5143 controlling much of the finer details of a G76 cycle. Unfortunately, I didn't have the inclination to spell it all out. Plus, I am not a good re-translator of Japanese to English. What they say in the book isn't always a clear picture of what the values in the parameters actually do. That's Fanuc-speak for you. Good luck.

  5. #5
    Join Date
    Mar 2010
    Posts
    166
    Thanks
    0
    Thanked 17 Times in 16 Posts

    Default Re: g76 threading cycle (2 block g76)

    As per 0i parameter manual, 0001#1 (FCV) selects between series 0 format (series 16/18 compatible format) and series 10/11 format. There are references to FS15, but it is not explained how to select this format. Any idea?

  6. #6
    Join Date
    Jul 2010
    Posts
    5
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: g76 threading cycle (2 block g76)

    thanks , what i,m gathering is that the 2 line format gives u 6 infeed angles
    only in one direction. that should be ok, i will try the one it calls out for the angle i need. i tried the 2 line format on the machine and seemed to
    work ok. ( with out cutting a chip) i should be cutting chips soon tho

  7. #7
    Join Date
    Mar 2010
    Posts
    166
    Thanks
    0
    Thanked 17 Times in 16 Posts

    Default Re: g76 threading cycle (2 block g76)

    The following example of 2-block G76 would be helpful. It makes M30 thread of 30 mm length:

    O0008
    G21 G97 G98
    G54
    G28 U0 W0
    T0707
    M03 S200
    G00 X32 Z10
    G76 P031560 Q150 R0.15
    G76 X25.706 Z-30 P2147 Q250 F3.5
    G28 U0 W0
    M05
    M30

    The threading cycle in this program is based on the following parameters:
    Number of finishing passes = 3
    Chamfer distance = 1.5 3.5 = 5.25 mm (3.5 mm is pitch)
    Thread angle (tool-tip angle) = 60 degree
    Minimum depth of cut = 150 micron = 0.15 mm
    Finishing allowance (on dia.) = 0.15 mm
    Core diameter = 25.706 mm (from threading chart)
    Axial end of thread = 30 mm in the negative Z−direction
    Depth of thread = 2147 micron = 2.147 mm (from threading chart)
    First depth of cut = 250 micron = 0.25 mm
    Lead (= pitch, for single-start) = 3.5 mm

    There is also a provision for an R-word in the second block of G76 for taper threads.

  8. #8
    Join Date
    Sep 2009
    Location
    Delhi, INDIA
    Posts
    33
    Thanks
    0
    Thanked 1 Time in 1 Post

    Default Re: g76 threading cycle (2 block g76)

    Hi steelman,
    I know that what you wants to know.

    If you select 'P021560' threads goes to single side entering in threads profile.

    If you select 'P021500' threads goes to streight entry like G92 code style.

    If you select 'P021530' or P021529' threads goes to small zigzag type in z axis style.

    If you select 'P021520' threads goes to another big zigzag type style.

    You can change angles and see results.

    This not only thread angle but can change style also.

    Naval Chauhan
    Last edited by nvlchauhan; 08-26-10 at 04:54 AM.

  9. #9
    Join Date
    Jun 2012
    Posts
    6
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: g76 threading cycle (2 block g76)

    Quote Originally Posted by nvlchauhan View Post
    Hi steelman,
    I know that what you wants to know.

    If you select 'P021560' threads goes to single side entering in threads profile.

    If you select 'P021500' threads goes to streight entry like G92 code style.

    If you select 'P021530' or P021529' threads goes to small zigzag type in z axis style.

    If you select 'P021520' threads goes to another big zigzag type style.

    You can change angles and see results.

    This not only thread angle but can change style also.

    Naval Chauhan
    This is not what the OP is asking. The older single block G76 cycle has the option of programming P1, P2, P3 or P4. These values are:

    P1: One-side cutting with constant cutting amount
    P2: Zigzag cutting with constant cutting amount
    P3: One-side cutting with constant cutting depth
    P4: Zigzag cutting with constant cutting depth


    I can find no reference to the fact that changing the compound infeed angle on the 2-block call will change anything other than the compound infeed. 20 is not a valid value. Only 0, 29, 30, 55, 60 and 80 are valid numbers for the 2-block call. The 1-block call uses an A to specify the compound infeed, and any angle can be commanded between 0 and 120 degrees in 1 degree increments.

Similar Threads

  1. Auto operation cant cycle start alarm occurs when cycle start is pushed.
    By Petro in forum General CNC & Manufacturing Discussion
    Replies: 1
    Last Post: 10-10-12, 10:28 AM
  2. G78-threading cycle help please
    By CHANDRU in forum Programming / Applications
    Replies: 4
    Last Post: 07-01-12, 06:08 PM
  3. Want Buy CNC Threading Machines and Setting up an API Threading Workshop
    By delta in forum General CNC & Manufacturing Discussion
    Replies: 3
    Last Post: 12-27-10, 05:26 AM
  4. No solution of block end alaram
    By balamurugan in forum Fanuc Controls
    Replies: 1
    Last Post: 08-09-10, 12:20 PM
  5. Starting Program At N Block
    By chucker in forum Programming / Applications
    Replies: 2
    Last Post: 11-23-09, 01:39 AM

Posting Permissions

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