PDA

View Full Version : peck drilling on mach 3



Crazy L
18-02-2018, 08:14 PM
Hi guys

Quick question. I have a small desktop mill running Mach 3 and when I wrote a small prog earlier using G83, with 4 holes to drill, it drilled the 1st one, but simply went to the next positions without drilling in those positions.

Any ideas on what I'm missing here? Cheers guys.

JAZZCNC
18-02-2018, 09:17 PM
Hi guys

Quick question. I have a small desktop mill running Mach 3 and when I wrote a small prog earlier using G83, with 4 holes to drill, it drilled the 1st one, but simply went to the next positions without drilling in those positions.

Any ideas on what I'm missing here? Cheers guys.

Need to see the code.!!

magicniner
19-02-2018, 07:58 AM
A thought did strike me, could be irrelevant but if the code is good, what Version of Mach3 are you using?

Crazy L
19-02-2018, 01:24 PM
Hi guys, code is thus:

G0 X-12.5 Y0.
G83 G98 Z-9. R2. Q1. F50
G0 X0. Y12.5
X12.5 Y0.
X0. Y-12.5

Like I said, goes to position and drills 1st hole, not the other 3.

No idea what version I'm running tbh and can't find out until I get home tonight, it was on the pc when I bought it as a running machine.

magicniner
19-02-2018, 01:41 PM
You've put a G0 on line 3 of that code
It shouldn't be there, just X/Y coordinates for further points at which to peck drill.
I believe there is also a specific G code to define the end of the canned cycle but would have to look that up,
Regards,
Nick

Crazy L
19-02-2018, 01:46 PM
Ok thanks, but I'm not sure if that G0 is there in reality as I'm only trying to recall what I have written.

If I have left it there I shall delete it and see where it gets me. Many thanks.

I use heidenhain at work and have not touched fanuc in 10 years so Im a bit rusty.

Crazy L
19-02-2018, 01:47 PM
G80 usually cancels canned cycles

magicniner
19-02-2018, 01:57 PM
Ok thanks, but I'm not sure if that G0 is there in reality as I'm only trying to recall what I have written.

If I have left it there I shall delete it and see where it gets me. Many thanks.

I use heidenhain at work and have not touched fanuc in 10 years so Im a bit rusty.

Without the line 3 G0 it works on my test copy of Mach3 - I have a clone of my live Mach3 install and config on my laptop (less the PP driver and limit/home switch config), it's Mach3 R3.043.062

Neale
19-02-2018, 03:50 PM
The reason for the problem is that the 2nd set of coordinates is given with a G0, and the next two sets do not have any "G" command. Giving a set of coordinates without a "G" command means "repeat the last G0/G1/G83/whatever using these coordinates". So you move to the second location using G0, do nothing there, and then, in effect, do two more G0 commands. Nick is quite right - drop the G0 in line 3 but leave the coordinates as given, and you will then execute the three further peck drill cycles. Don't need to bother with ending the cycle.

Crazy L
19-02-2018, 07:02 PM
Hey guys, came home and fired up the pc to have a nosey at my prog, and yes, there was a G0 in there. I have removed it and it drills all the holes now. Ta muchly chaps.

After 12 hrs of cutting metal, its now time to...cut metal.