Reply with QuoteI do not think it can be done with G74. Does your machine have G83 enabled? If not, does it have macros enabled? You can write your own macro.
G74 peck drilling
We were trying to use G74 to drill a hole about 8inches deep on a cnc lathe that has a Fanuc 11 T controller.We need the drill to pull ALL the way out of the hole on each peck.
What info goes on the G74 line to make it pull all the way out of the hole on each peck?
Thanks, Hacky
Similar Threads:
I do not think it can be done with G74. Does your machine have G83 enabled? If not, does it have macros enabled? You can write your own macro.
txcncman is right, G74 just does a short chip breaking retract and doesn't go the whole way.
If you don't have a cycle that has a full retract you can use our g-code wizard to generate the code for a custom cycle that does just about anything you want in a custom cycle using simple G01 moves.
It's free during beta test. Sign up form is here:
CNC Conversational Programming Software from G-Wizard
Cheers,
BW
Try G-Wizard Machinist's Calculator for free:
http://www.cnccookbook.com/CCGWizard.html
Will these help?
Al.
CNC, Mechatronics Integration and Custom Machine Design
“Logic will get you from A to B. Imagination will take you everywhere.”
Albert E.
Thanks for the replies. The lathe is an 80's toyoda , and the guy who runs it says it is not G83 enabled. He also said it wont do macros either. So he just did it with G01 and G0 moves. But, just in case I will try and print out what Al The Man sent.
Thanks again guys!
hackmeister
You can try this G74 X0.0Z-1.0 D.125 L.250 F.005
( Z ) being the max depth ( D ) is the peck ( L ) is a full retract after it has gone .250 deep ( F ) feed
Put your own numbers, There is many ways to do this,try this first
A G83 is mostly used for milling so won't be available for your Fanuc 11 lathe control
Mactec54
Does your control have the ability to do looping with subs? The following should drill a hole 2.400 deep.
%
.....
G00 X0. Z0.1
M98 P1001 L20
G00 Z0.1
.....
%
%
O1001
G1 W-0.125 F0.004
G0 W3.
G0 W-2.975
M99
%
11T control supports Macro programming, but is an option that has to be paid for first. Too bad you don't have the option as I have a nice little subprogram that does what you are looking for....in Macro B.
EDIT: If you try txcncman's example, make sure you have 3 inches of clearance behind the turret when the drill is in front of the part. Hitting a subspindle or tailstock is to be avoided.
Re: G74 peck drilling
Wow. Cabin fever must be rampant.This is a 6 year old thread. The Hardinge 9135 program Al referred to was replaced by 9136 a long time ago. The OP couldn't use either because he didn't have Macro B.
I would have a problem with several things with the above G74 sample. First: three M-codes are allowed in the same block....if your control supports it. I've yet to run a lathe with a Fanuc control that did. Second: Fanuc manuals and the lathe manuals I've seen all show the feedrate in the second G74 block. Now it is possible that the control will pick up the last feedrate in that operation, but why would you want to look through your program to find it when it could be right there in the G74 block? Third: X0 is used to position the tool before the G74 call and therefore does not need to be in the call. Fourth: I consider the absence of a decimal point for the Z-value to be poor form. Same for the R.
I am aware that if no decimal point is used, the control reads the number from right to left. However, I've never tried it with the R-value, so I have no idea what the control will do about the absence of a decimal point. I program in inch, not metric. I believe a standard metric lathe is programmed with 3 values after the decimal point. In the above sample there would be no pecks so why use a G74? The peck would be 15.000 while the drill depth is .07
Now I know of one control that would read Z70 as Z70. but it is not a Fanuc control.
Re: G74 peck drilling
I have had the same problem since CNC Masters up dated the controller and software on my 1440 lathe. When I tried the G83 that worked before it did not work. I asked Omar at CNC MASTERS about this and was told that the old controller allowed it because of a work-around with the old controller. BUT he would look into a new wizard.Originally Posted by hackmeister
I just got a software update today with the new wizard that allows full retract and peck depth just like G83 for mills. They are very accomodating. I suggested another change to the thread wizard that would add "spring pass" to the cycle. And they added that to. It can now make 3 passes at the last depth.
I have been very happy with this company and the support offered long after the warranty period. I've had the lathe for 5 years and it is still doing great work. They are developing a closed loop system with DRO. I'm sure it will be great to.
