547,586 active members*
1,383 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > G-Code Programing > Rapid to (# set by Parameter) What's yours?
Results 1 to 10 of 10
  1. #1
    Mfg Engineer
    Join Date
    Nov 2003
    Posts
    459

    Rapid to (# set by Parameter) What's yours?

    During G83 peck drilling rapid motion returns to +____

    This positive distance from the last feed depth is set by a parameter on your Fanuc control.
    #532 on an OM control
    This parameter is set by most factorys at 1000
    or .100 thousands
    That is way too much if you are drilling with small drills.
    Smaller drills are programmed at lower feeds and the time wasted, feeding thru air can really add up.

    If you do much drilling at all, check this setting...
    Before you do, get a cycle time of commonly drilled holes and see how much time you'll end up saving, you'll be amazed!

    I think this setting should be set at 200
    or .020 thousands
    or 100 (.010)

    The Fadal control uses a P_ value to set this distance in the G83 line of code.
    Fadal default is zero. This means that Rapid motion returns to the last peck depth. I believe a little clearance here is best in the event of a chip falling back in the hole... I use P.010

    Scott_bob

  2. #2
    Registered
    Join Date
    Mar 2003
    Posts
    106
    I use .020 for the rapid return. The boss says I should use .005 to .010 to reduce the cycle time. Let's see, a drill moving at 8.5 IPM will move the extra .010 in about 1/15th of a second. Not much savings there compared to a tool breaking and the time it takes to replace and re-set the tool.

  3. #3
    Mfg Engineer
    Join Date
    Nov 2003
    Posts
    459
    E-stop,

    Do you know what your CNC was set at the factory?

    Scott_bob
    Scott_bob

  4. #4
    Registered
    Join Date
    Mar 2003
    Posts
    106
    Yes. The factory setting was .050, which is a good, safe place to start.

  5. #5
    Registered
    Join Date
    Jul 2004
    Posts
    2
    E-Stop,
    0.05 is fine, If you want to save time invest into some premium drills that cut faster.

  6. #6
    Registered
    Join Date
    Jul 2008
    Posts
    6

    peck drilling not possible

    dear friends

    i have a Fanuc Oi Mate Series control on my VMC.

    i want to drill 50 mm deep drill with 5 pecks.i have used G83 but its not working.

    please tell me which parameter to edit to start the peck drilling.

    its really urgent i am loosing my 50% extra time in drilling.

    thanks
    Suraj.

  7. #7
    Gold Member
    Join Date
    Mar 2003
    Posts
    2932
    What do you mean "it's not working"? What does it do? Do you get an alarm? If so, what alarm? Does it drill but not peck? Post your G83 line here so maybe we can help you.

  8. #8
    Registered
    Join Date
    Jul 2008
    Posts
    6

    hi

    hi

    thanks for replying.

    the problem was no pecks during drilling.

    but i found the parameter by myself

    its 5114

    i have one more problem. please let me know how to use to coordinate codes like G54 and G55, G56, G57 In same program in absolute G90 cycle to use different origin.

    thanks.

  9. #9
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    It's very easy to do. You set the G54-G59 to the position that you want to reference. Take the machine position numbers of were you want to orgin and put them in the work coordinates G54-G59. Say it is in G55...now all you have to do is make sure you use G55 in your program. G0G90G55X0Y0.

    These will act as any other G-code. They stay modal until changed or rest of the control. Most Fanucs default back to G54 when reset.

    Stevo

  10. #10
    Mfg Engineer
    Join Date
    Nov 2003
    Posts
    459

    Re: Rapid to (# set by Parameter) What's yours?

    When the "Rapid to delta distance" to the last feed depth is set too high!
    Time is wasted feeding thru air. Depending on how much distance your machine is set for in Fanuc Parameter #5114 (G73) & #5115 (G83), there is a lot of cycle time to be gained!!! Time is money...
    If you are drilling with small peck amounts it really adds up to a lot of time!

    Example: .040 Diameter Drill, Peck: Q.020 and you are drilling .50 deep
    Over 1/2 of your cycle time is wasted feeding thru air. (We once saved 40 hours of machine time, just by setting our #5115 to .010" from the factory setting of .10") No joke!
    This is pure $ wasted! Don't ignore this simple solution to cycle time reduction!

    Try your own Parameter setting trial and post your results...
    Scott_bob

Similar Threads

  1. Haas rapid parameter, and offset param?
    By underthetire in forum Haas Mills
    Replies: 2
    Last Post: 06-23-2012, 12:42 AM
  2. Rapid speed parameter M32
    By MIKEL12 in forum Mazak, Mitsubishi, Mazatrol
    Replies: 2
    Last Post: 10-08-2010, 10:41 PM
  3. Rapid on X Parameter - HAAS TL-1
    By Bosarge66 in forum Haas Lathes
    Replies: 0
    Last Post: 08-11-2010, 08:44 PM
  4. Rapid speed parameter in a ES-L6 with OSP U10L?
    By aaroncswenson in forum Okuma
    Replies: 6
    Last Post: 05-17-2010, 03:24 PM
  5. Please help with feed/rapid override parameter
    By Hermle UWF851 in forum Fanuc
    Replies: 2
    Last Post: 04-22-2009, 10:29 PM

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
  •