584,830 active members*
5,831 visitors online*
Register for free
Login
Results 1 to 11 of 11
  1. #1
    Join Date
    Dec 2009
    Posts
    22

    G74 peck drilling

    We were trying to use G74 to drill a hole about 8inches deep on a cnc lathe that has a Fanuc 11 T controller.We need the drill to pull ALL the way out of the hole on each peck.
    What info goes on the G74 line to make it pull all the way out of the hole on each peck?
    Thanks, Hacky

  2. #2
    Join Date
    May 2004
    Posts
    4519
    I do not think it can be done with G74. Does your machine have G83 enabled? If not, does it have macros enabled? You can write your own macro.

  3. #3
    Join Date
    May 2005
    Posts
    2502
    txcncman is right, G74 just does a short chip breaking retract and doesn't go the whole way.

    If you don't have a cycle that has a full retract you can use our g-code wizard to generate the code for a custom cycle that does just about anything you want in a custom cycle using simple G01 moves.

    It's free during beta test. Sign up form is here:

    CNC Conversational Programming Software from G-Wizard

    Cheers,

    BW
    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html

  4. #4
    Join Date
    Dec 2003
    Posts
    24216
    Will these help?
    Al.
    Attached Thumbnails Attached Thumbnails Drill_peck_macro.jpg   Drill_peck_macro2.jpg  
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  5. #5
    Join Date
    Dec 2009
    Posts
    22
    Thanks for the replies. The lathe is an 80's toyoda , and the guy who runs it says it is not G83 enabled. He also said it wont do macros either. So he just did it with G01 and G0 moves. But, just in case I will try and print out what Al The Man sent.
    Thanks again guys!

  6. #6
    Join Date
    Jan 2005
    Posts
    15362
    hackmeister

    You can try this G74 X0.0Z-1.0 D.125 L.250 F.005

    ( Z ) being the max depth ( D ) is the peck ( L ) is a full retract after it has gone .250 deep ( F ) feed

    Put your own numbers, There is many ways to do this,try this first

    A G83 is mostly used for milling so won't be available for your Fanuc 11 lathe control
    Mactec54

  7. #7
    Join Date
    May 2004
    Posts
    4519
    Does your control have the ability to do looping with subs? The following should drill a hole 2.400 deep.

    %
    .....
    G00 X0. Z0.1
    M98 P1001 L20
    G00 Z0.1
    .....
    %

    %
    O1001
    G1 W-0.125 F0.004
    G0 W3.
    G0 W-2.975
    M99
    %

  8. #8
    Join Date
    May 2007
    Posts
    1003
    11T control supports Macro programming, but is an option that has to be paid for first. Too bad you don't have the option as I have a nice little subprogram that does what you are looking for....in Macro B.

    EDIT: If you try txcncman's example, make sure you have 3 inches of clearance behind the turret when the drill is in front of the part. Hitting a subspindle or tailstock is to be avoided.

  9. #9
    harshal Guest

    Re: G74 peck drilling

    FOR DESCRIPTION CLICK HERE Peck drilling cycle for turning (G74 cycle) - CNC PROGRAMMING TUTORIAL
    04534
    N10 G90 G21 G99 F0.15 ;
    N20 M06 T05 05 ;
    N30 M03 G97 S500 ;
    N40 M08;
    N50 G00 X0 Z2 ;
    N60 G74 R1 ;
    N70 G74 X0 Z-70 Q15000 ;
    N80 G00 X150 Z150 ;
    N90 M05 M09 M30 ;

  10. #10
    Join Date
    May 2007
    Posts
    1003

    Re: G74 peck drilling

    Wow. Cabin fever must be rampant. This is a 6 year old thread. The Hardinge 9135 program Al referred to was replaced by 9136 a long time ago. The OP couldn't use either because he didn't have Macro B.

    I would have a problem with several things with the above G74 sample. First: three M-codes are allowed in the same block....if your control supports it. I've yet to run a lathe with a Fanuc control that did. Second: Fanuc manuals and the lathe manuals I've seen all show the feedrate in the second G74 block. Now it is possible that the control will pick up the last feedrate in that operation, but why would you want to look through your program to find it when it could be right there in the G74 block? Third: X0 is used to position the tool before the G74 call and therefore does not need to be in the call. Fourth: I consider the absence of a decimal point for the Z-value to be poor form. Same for the R.

    I am aware that if no decimal point is used, the control reads the number from right to left. However, I've never tried it with the R-value, so I have no idea what the control will do about the absence of a decimal point. I program in inch, not metric. I believe a standard metric lathe is programmed with 3 values after the decimal point. In the above sample there would be no pecks so why use a G74? The peck would be 15.000 while the drill depth is .07

    Now I know of one control that would read Z70 as Z70. but it is not a Fanuc control.

  11. #11
    Join Date
    Mar 2006
    Posts
    51

    Re: G74 peck drilling

    Quote Originally Posted by hackmeister View Post
    We were trying to use G74 to drill a hole about 8inches deep on a cnc lathe that has a Fanuc 11 T controller.We need the drill to pull ALL the way out of the hole on each peck.
    What info goes on the G74 line to make it pull all the way out of the hole on each peck?
    Thanks, Hacky
    I have had the same problem since CNC Masters up dated the controller and software on my 1440 lathe. When I tried the G83 that worked before it did not work. I asked Omar at CNC MASTERS about this and was told that the old controller allowed it because of a work-around with the old controller. BUT he would look into a new wizard.

    I just got a software update today with the new wizard that allows full retract and peck depth just like G83 for mills. They are very accomodating. I suggested another change to the thread wizard that would add "spring pass" to the cycle. And they added that to. It can now make 3 passes at the last depth.

    I have been very happy with this company and the support offered long after the warranty period. I've had the lathe for 5 years and it is still doing great work. They are developing a closed loop system with DRO. I'm sure it will be great to.

Similar Threads

  1. Combining peck drilling cycle with deep hole peck
    By adams4182 in forum G-Code Programing
    Replies: 3
    Last Post: 07-28-2013, 09:07 PM
  2. Peck drilling on a 16/18i?
    By TheMoose in forum Fanuc
    Replies: 24
    Last Post: 09-09-2008, 09:34 PM
  3. Peck Drilling Help
    By soonervols in forum G-Code Programing
    Replies: 15
    Last Post: 06-09-2008, 12:26 PM
  4. v22 peck drilling
    By 68sixspeed in forum BobCad-Cam
    Replies: 7
    Last Post: 04-03-2008, 10:17 PM
  5. Peck Drilling
    By RBrandes in forum Haas Mills
    Replies: 10
    Last Post: 06-19-2007, 01:03 AM

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
  •