Hello Guest it is May 08, 2021, 03:49:50 PM

Author Topic: Peck Drilling....  (Read 12672 times)

0 Members and 1 Guest are viewing this topic.

Peck Drilling....
« on: December 25, 2009, 12:00:42 AM »
Are there any good rules of thumb for setting the Q parameter when peck drilling?  It seems to me this probably should vary with hole depth, doing shorter pecks as the hole gets deeper, but there is no provision in G73/G83 for doing that.

Regards,
Ray L.
« Last Edit: December 25, 2009, 12:03:06 AM by HimyKabibble »
Regards,
Ray L.

Offline comet

*
  •  325 325
    • View Profile
Re: Peck Drilling....
« Reply #1 on: December 25, 2009, 07:35:07 AM »
Ray,
  thats very true,you could drill the same hole with two or three G83's but alter the starting point
Re: Peck Drilling....
« Reply #2 on: December 25, 2009, 07:39:53 AM »
you could always mod the program yourself, adding G0 and G1 commands to suit your requirements.

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: Peck Drilling....
« Reply #3 on: December 25, 2009, 10:03:08 PM »
Ray,
I don't know of  any rules of thumb. You may want to have a look at the macros Melee posted for the lathe and the mill. Have yet to test them on the Mill but both of them worked great on the lathe. I was peck drilling little holes ( 0.020" with a silly .002" peck ). What I was trying to do was create the equivilant of a dwell time so the drill could just break the surface for a start. BTW, those macros allow you to drill a number of holes and not just one.
The only thing is you can't just use them from the MDI as they need to be in a file.
RICH
Re: Peck Drilling....
« Reply #4 on: December 25, 2009, 10:15:35 PM »
Ray,
I don't know of  any rules of thumb. You may want to have a look at the macros Melee posted for the lathe and the mill. Have yet to test them on the Mill but both of them worked great on the lathe. I was peck drilling little holes ( 0.020" with a silly .002" peck ). What I was trying to do was create the equivilant of a dwell time so the drill could just break the surface for a start. BTW, those macros allow you to drill a number of holes and not just one.
The only thing is you can't just use them from the MDI as they need to be in a file.
RICH

Where would I find those macros?

I just finished writing my own G-code generator for peck cycles, based on drill bit information from Irwin.  RPM, feed, and peck depth all vary based on depth.  If I get time tomorrow, I'll try them on the machine.

Regards,
Ray L.
Regards,
Ray L.

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: Peck Drilling....
« Reply #5 on: December 26, 2009, 08:12:17 AM »
Ray,
Here is the link and in the download there is a read me file on the macro's. May also just take a quick read of the
thread.

http://www.machsupport.com/forum/index.php/topic,13400.msg88226.html#msg88226

RICH
Re: Peck Drilling....
« Reply #6 on: December 26, 2009, 11:48:16 AM »
Ray,
Here is the link and in the download there is a read me file on the macro's. May also just take a quick read of the
thread.

http://www.machsupport.com/forum/index.php/topic,13400.msg88226.html#msg88226

RICH

Yeah, those macros look quite comprehensive, though I don't care for the trick he uses to get the parameters from the G-code file.  I will study them to see how he arrives at peck depths, etc.

Regards,
Ray L.
Regards,
Ray L.
Re: Peck Drilling....
« Reply #7 on: December 27, 2009, 08:33:57 AM »
Ray,

Please enlighten me a little more about this...

The G83 (deep hole peck cycle) and G73 (high speed peck cycle) seem to work similarly in milling where Q is concerned. That's why I don't understand. I have always used very shallow pecks when the hole must be very accurate. The last peck is shortened to accommodate the total depth as in: N8 G73 G99 R-0.4315 Z-0.7463 F3.0 Q0.0150 X0.0000 Y0.3937 - the last peck (Q) is .0148". The difference as I see it for the use of G83 over G73 is the retract amount and that is also determined by the chip formed by the material being drilled - such as steel and a long curl chip can use G73 since the chip will extract itself so the retract does not need to totally exit the hole as with G83.

Or have I missed your question totally...?

Thanks,
Bill C.
« Last Edit: December 27, 2009, 09:31:54 AM by BClemens »
Re: Peck Drilling....
« Reply #8 on: December 27, 2009, 10:58:02 AM »
Ray,

Please enlighten me a little more about this...

The G83 (deep hole peck cycle) and G73 (high speed peck cycle) seem to work similarly in milling where Q is concerned. That's why I don't understand. I have always used very shallow pecks when the hole must be very accurate. The last peck is shortened to accommodate the total depth as in: N8 G73 G99 R-0.4315 Z-0.7463 F3.0 Q0.0150 X0.0000 Y0.3937 - the last peck (Q) is .0148". The difference as I see it for the use of G83 over G73 is the retract amount and that is also determined by the chip formed by the material being drilled - such as steel and a long curl chip can use G73 since the chip will extract itself so the retract does not need to totally exit the hole as with G83.

Or have I missed your question totally...?

Thanks,
Bill C.

AFAIK, the *only* difference between G73 and G83 is how far it retracts between pecks - G73 retracts fully to the R plane, while G83 only retracts a small amount from the previous depth.  Neither does any of the optimization required for drilling deep holes -  reducing RPM, feedrate, and peck depth as the hole goes beyond about 3 diameters deep.  That is what I'm after, and seem to have achieved.  G73 and G83 also require manually programming the proper peck depth, or programming multiple cycles, to get a clean bottom-side on thru-holes by having the next-to-last peck break partway through the bottom surface, then doing a final peck, with dwell, to finish the hole without a burr on the exit side.  Mine now does that automatically, by adjusting the final, and next-to-final peck depths as required.

Regards,
Ray L.
Regards,
Ray L.
Re: Peck Drilling....
« Reply #9 on: December 27, 2009, 12:00:26 PM »
Are these macros developed by Hardinge of any help?
Nosmo.