G83 Canned Cycle- Fanuc 18-T Control

I'm hopeing someone can explain a problem I'm having with a G83 Canned Cycle on a Daewoo Puma lathe with a Fanuc 18-T control. Below is a copy of the program.

N5(1.0" SPADE DRILL)
G30 UO. W0.
G97 S153 M3
T0505
G99 G00 G54 Z1.0 M8
X0.0
G83 Z-6.25 R0.1 Q4000 F0.008
G0 Z1.0
X12.0 M9
G30 U0. W0.
M01

The problem I'm having is that the tool comes down to X0 Z1.0 and then rapids back to Z1.10 and starts feeding from there. I've tried positioning the tool at Z0.1, but then the tool will rapid back to Z0.2 and start feeding from there instead of Z0.1. I've also tried putting a G99 and G98 seperatatly in front of the G83 with the same results. Any ideas as to why the tool will not start feeding at Z0.1? Any help would be greatly appreciated! Also, great site!

Regards,

On a lathe your R plane is incremental distance from your start point. so you would need

G83 Z-6.25 R-.98 Q4000 F0.008

that would start drilling at Z.02

Why is there a G99 after T0505?

N5(1.0" SPADE DRILL)
G30 UO. W0.
G97 S153 M3
T0505
G00 G90 G54 X0. Z1. M8
Z.1
G98 G83 Z-6.25 R0.1 Q4. F0.008
G80
G0 Z1.0
X12.0 M9
G30 U0. W0.
M01

I pasted your program and made a few changes. Should work.

Also, you did not cancel your G83 either (G80).

Hope it works for ya.

Izzoe

G99 is feed/rev. Probably there as a precaution.
And that Q4000 is actually Q.4

Sakis

Never seen a lathe or anything for that matter with incremental R. Then again, never seen a Daewoo either.
Having said that, that's exactly what it looks like

I've never seem a incremental R plane either! The Q is actually correct, it has to be in a non-decimal format.

Daewoo, puma, kia, hyundai, all suck. there code does not read the same as reagular fanuc. the machine tool builder changes small things in the code that doesnt seem significant but screws up the whole machine. getting tech support takes an act of congress. I have a kia/hyundai 21lms and i have never ran a bigger peice of sh%% in my life.

I was told that you don't need to put in a G80 after the canned cycle to cancel it because it does it automatically.

Hey!

I'll match you any day on which machine is a bigger piece of sh%%! My Daewoo vs. your Kia/Hyundai. I just can't believe people but this junk!

Guys, is this a full-moon thing?
I mean shoudn't you be arguing who's is better, bigger, more etc?

G80 isn't necessary but nice to have there.

use a g83 daily on my 18t

its position and drill no r value

eg.

g97 s175 m3
g0 x0.0 z.1 m8
g83 z-x.xxx q4000 f.003
g0 z.3 m9


no g80 needed.

Are we talking Live tooling Here?

The "R" tells the tool to move by that much in that direction from the position before the G83 line. So, you went to Z1.0 with an R.1 (positive) so the tool moved in the positive direction by .1 which is Z1.1 and then started feeding.If you have spotted the hole you may want the "R" to be "R-.1" then the tool will rapid from "Z1.0" to "Z.9" and start drilling from there. When each peck depth is reached it will pull out to "Z1.0". This is useful when you have a counterbore or a larger hole at the begining and want to rapid closer to the bottom of the first hole but still rapid out of the part after each peck.

cogsman

R defines the plane to which drilling starts, and the point to which the drill retracts to between pecks. So in the case you've mentioned the drill should retract to Z1.1 and not Z1.0. So the argument of retracting above the starting point is mute, as you'll be drilling air for the first peck.
With that said, having R as incremental makes absolutely no sense. I understand that this is on a lathe, but it still should be exactly like on the mill. Why would you position your drill to the Z clearance point, and then calculate the incremental distance from there to the point where you want to start drilling from? R should be absolute to the part, just like every other programmed dimension. Why is it better to figure Z - R as to the starting point instead of Rabsolute, I have no idea.
HAAS has a setting where you can set a distance to retract to above the R plane. This unfortunately is not accessible from within the program. Now if they can only add another modifier to the G83 line <say I value> and change it on the fly, it would be the cat's meow.

Here is a description right out of the book. This is for a Mitsubishi control.

G83-(option) Peck drilling cycle. There are (2) parameters related to G83.
Param #5101 bit2 "High speed" if "0" then the pecks do NOT come out of
the hole, they only back up the amount of Param #5114 "G83 Retract",
to break the chip and then start feeding again.

Param #5114 "G83 Retract -200" is the amount to rapid back into the
hole from the last peck for clearance.

I suggest...
Param #5101 bit2 = "1" -Rapid out of hole every peck.
Param #5114 "G83 Retract" = "-200" =-.02 from last peck. No decimal.

Example-
G0 Z-.05 T22
G83 Z1. F.001 R.03 Q0400 P0

Z1. =Z position of the bottom of the hole

F.001 =Feed in IPR or IPM

R.03 =Rapid from current Z position the R amount incrementally.
If starting at Z-.05 and R=.03 then the Z axis rapidly
positions to "Z-.02" and after every peck Z retracts to
the same position "Z-.02". If you use "R-.03" it is the same
as "R.03"

Q0400 =Peck amount -same as .04 but not allowed a decimal point

P0 =Dwell amount at the bottom of the hole. You can just leave
P off the command line if you want

Heinz may want to stop by and say something here, but I think standard Fanuc uses G73 as the high speed peck drilling cycle, where the tool does not retract to the R plane. G83 is just what it is, start from and retract to R.
What you're showing from the Mits is actually 2 different codes on a Fanuc.

But then again, it still doesn't make sense to me to use R as incremental.

There is no G73 high speed peck cycle on Fanuc lathes. G73 is a Turning cycle.