Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: HimyKabibble 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.
-
Ray,
thats very true,you could drill the same hole with two or three G83's but alter the starting point
-
you could always mod the program yourself, adding G0 and G1 commands to suit your requirements.
-
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
-
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.
-
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
-
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.
-
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.
-
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.
-
Are these macros developed by Hardinge of any help?
Nosmo.
-
These are for lathe use. OK, I'll catch up - I'm still drilling vertically on a mill.
Thanks,
Bill C.
-
Are these macros developed by Hardinge of any help?
Nosmo.
Those are interesting. I'm surprised by the aggressive start, but the rest is consistent with my understanding and experience. I haven't had much luck with drilling 3 diameters in one pass on either small or large drills. It works OK in the mid-range - perhaps 1/8-5/16 or so.
Regards,
Ray L.
-
It works every time if you do it by accident!
Bill C.
-
Ray,
When are you going to post your macros and will they work on the lathe?
RICH
-
Ray,
When are you going to post your macros and will they work on the lathe?
RICH
Rich,
What I wrote is not Mach3 macros, but a G-code generator, written in Perl, that's part of the post-processor I wrote to optimize the G-code for my machine. Unfortunately, there's no clean way to pass more than 3 arguments to a Mach3 VB macro (only P, Q, and R are accessible), and peck drilling requires more than 3 arguments. I've asked Brian to fix this in v4, so we'll be able to have ALL arguments in macros (X-Z, A-C, S, F, P, I, J, R, Q, etc.).
Regards,
Ray L.
-
If you find some good info on pecking remember to post it here. I didn't do a search and surely there is some good advice out there. What I did was tailor the parameters to mimic what worked when doing it manualy ,but then,
that was for real small holes. Learning never stops.
RICH
-
Melee,
I'm just using a lookup table. Basically run full RPM and feed, and run a peck depth of one diameter, until 3 diameters, then reduce feed and peck depth by 10% and RPM by 5% for each additional diameter below that up to 6 diameters. Seems to work OK, but it's had very little testing to date. I found an Irwin drill spec sheet that suggested something similar.
I understand completely why you parsed the line as you did, and it was a very clever solution to an otherwise rather intractable problem. I've just found such solutions tend to be rather fragile over time (that, and I can't think of worse language than VB to have to write a parser in....). But, obviously, you had no choice here. It was also what prodded me to ask Brian to make all arguments available, so a good thing will come from it for sure. My solution was to just expand the G73 into G-code using a post-processor, for which I already had a working parser, so it was trivial to implement.
Regards,
Ray L.
-
Hi again Ray,
I have written an amended version of my high speed pecking macro, which allows for variable pecking as the hole deepens, using your rule of thumb as per previous post.
A debug print of the internal lookup table it creates, shows the results when drilling a ridiculously deep hole with a 4.5mm drill in simulation
4.5mm drill 600 RPM MaxPeck 4.5 MinPeck 1.5
Hole depth 51mm
Once either MinPeck is reached or 50% of original RPM, values are capped
Entry 0 Peck mm 4.5 Speed 600
Entry 1 Peck mm 4.5 Speed 600
Entry 2 Peck mm 4.5 Speed 600
Entry 3 Peck mm 4.05 Speed 570
Entry 4 Peck mm 3.64 Speed 541
Entry 5 Peck mm 3.28 Speed 513
Entry 6 Peck mm 2.95 Speed 487
Entry 7 Peck mm 2.65 Speed 462
Entry 8 Peck mm 2.39 Speed 438
Entry 9 Peck mm 2.15 Speed 416
Entry 10 Peck mm 1.93 Speed 395
Entry 11 Peck mm 1.74 Speed 375
Entry 12 Peck mm 1.56 Speed 356
Entry 13 Peck mm 1.5 Speed 356
Entry 14 Peck mm 1.5 Speed 356
Entry 15 Peck mm 1.5 Speed 356
Entry 16 Peck mm 1.5 Speed 356
Entry 17 Peck mm 1.5 Speed 356
Entry 18 Peck mm 1.5 Speed 356
Entry 19 Peck mm 1.5 Speed 356
Entry 20 Peck mm 1.5 Speed 356
Do you have any info re progressive reduction of feed rate?
It would seem sensible to reduce it in line with RPM or you are actually asking the drill to do more work per rev than previously.
What do you think?
regards
Melee
As I said, I reduce feedrate by 10% for each drill diameter in depth beyond 3, just as I do for peck depth. So, chipload actually decreases as you go deeper, since RPM is only decreasing at 5% per diameter. If you come up with any refinements on this, I'd love to hear about it. I've been unable to do much testing, due to electronic problems with my machine, awaiting some parts....
Regards,
Ray L.