Hello Guest it is July 08, 2020, 11:45:36 AM

Author Topic: G73, but not really G73  (Read 2062 times)

0 Members and 1 Guest are viewing this topic.

G73, but not really G73
« on: November 02, 2016, 12:04:32 PM »
Hey I have this program running.  And I am wondering if Mach3 interprets G73 correctly.  Drill is a .015 diameter, Pecking depth is set at .005, Minimum pecking depth is .005, Accumulated pecking depth is .0375, CHIP BREAK distance is .003 and no dwell.  This issue is that it seems the chip break distance isn't being taken into account so then the spindle retracts about .1, pulling the bit out of the hole, almost like a G83.  Is there another parameter I can manually input to force the Chip break distance or is this program correct and Mach3 doesn't jive?  BTW, it works this way whether I am using a .010 drill bit or a 3/8" drill bit at any length of hole.  Chip break isn't chip break.

(450-01631 WIRE HOLES 1)
N330 M5
N335 M9
N340 M1
N345 T78 M6
N350 S5000 M3
N355 G54
N360 M8
N370 G0 X0.3335 Y-0.216
N375 G43 Z0.6 H78
N385 Z0.2
N390 G73 X0.3335 Y-0.216 Z-0.0765 R0.01 Q0.005 F1.
N395 X0.4335
N400 Y-0.079
N405 X0.3335
N470 G80
N475 Z0.6
Re: G73, but not really G73
« Reply #1 on: November 04, 2016, 10:00:27 AM »
Come on somebody!!  Anyone have an idea what's up with G73 and Mach3?
Re: G73, but not really G73
« Reply #2 on: November 05, 2016, 09:13:43 AM »
Try this.

Go to Config, ports and pins, Mill options, G73 pull back dro.

Mike
We never have the time or money to do it right the first time, but we somehow manage to do it twice and then spend the money to get it right.

Offline Tweakie.CNC

*
  • *
  •  8,350 8,350
  • Super Kitty
    • View Profile
    • Tweakie.CNC
Re: G73, but not really G73
« Reply #3 on: November 05, 2016, 10:14:00 AM »
Try this.

Go to Config, ports and pins, Mill options, G73 pull back dro.

Mike

Excellent info Mike - something else I have learnt.

Tweakie.
KEEP SAFE !
Re: G73, but not really G73
« Reply #4 on: November 05, 2016, 12:17:36 PM »
Learning something everyday is the best way to keep the mind open.

As many things as I have learned from your posts Tweakie, I am glad to be able to teach you something.

Mike
We never have the time or money to do it right the first time, but we somehow manage to do it twice and then spend the money to get it right.
Re: G73, but not really G73
« Reply #5 on: November 05, 2016, 12:49:46 PM »
THANKS TOTALLYRC!

It worked!  It should make a significant change in time required especially when drilling a few hundred holes at a time.  


Again thanks,
Re: G73, but not really G73
« Reply #6 on: November 05, 2016, 01:08:51 PM »
On another note, I just figured out I can force the mill to chip break if I input a Dwell time period (even .001 sec) before retract.  The result is that it doesn't use a canned cycle, so a program of 25 lines to drill 6 holes, turns into a program that is 221 lines long instead to drill the same holes.  BTW, using HSMxpress.  So either way, use the Mach3 setting above or inputting a dwell time results in the same thing. 
Re: G73, but not really G73
« Reply #7 on: November 05, 2016, 08:52:33 PM »
Hi PW8697,
I am glad that it worked. I haven't tried it but if you have your CAM program output the code long hand the machine will probably cycle faster. When going from G00 to G01 MachX takes a finite amount of time to change modes. If the long hand code just uses a high feedrate instead of G00 it should be faster. I didn't really notice this "delay" until I got my "fast" machine running. One of the things I would like to investigate further after I am done prepping for winter.
We never have the time or money to do it right the first time, but we somehow manage to do it twice and then spend the money to get it right.