[trampus]

G73 X__Z__I__ K__D__L__F__E__T__

The "I" has me confused. It's my comprehendtion of certain words.
"The shift amount" in the X-axis direction. I understand the Z, but having a problem understanding this one. It is as simple as total X movement from the start of the first cutting feed rate to the end?
Thanks for reading.


:cheers:

[zooloader]

Using the I is something I've not used in G73.
A tapered groove diameterally could be achieved, I suppose, by using it.

It would normally be used when trepanning (G74 face grooving) instead of the K that you use in G73.

[littlerob]

I feel like the champion of "hijack" but that's not my intention. So if this post derails the OP just disregard it.

I like to keep my Canned cycles as uniform as possible so I use G85 for this (grooving) and a G82 ("trasnsverse shape design") instead of a G81 ("longitudal shape design"). For the beginning of shape design. In so doing you are going to use the same codes and the whole shop reads them the same. D,U,W,F.

IE, G85N***D.2U.05W.005F.02
N***G81(longitudal)

IE, G85N***D.05U.02W.005F.01
N***G82(transverse)

Robert

[trampus]

Thanks for your replies. I will be on this soon.
Then I'll know for sure.

[broby]

The "I" word is the distance the tool will move before retracting, or pecking, in the grooving cycle.
i.e. if you have a groove 10mm deep and you want to "peck" machine the groove by having the tool cut in 1mm at a time and then retract every 2mm you would use : I1 L2
If you do not want to use "Pecking" do not specify a value for I (or use I0)
I have scanned in a couple of pages from one of the manuals here.
Hope this helps.
Brian.

[zooloader]

@ broby,
I think you mean D1 L2. Looking at the scan the I is a rapid move from a clearance dia to where you want to start grooving/pecking from. The diagram doesn't make it very clear by drawing the I move the same length as the D moves.
Probably very handy if grooving behind a rib or shoulder or inside a larger groove:idea:

[broby]

Ah yes I do believe you are correct! Whoops on my behalf... good catch Zoolander.

[Algirdas Basher]

OHOHOHOHOHOHOH would ye look at that avatar, that shoulda been mine. :boxing:

Zoolander was that terrible Ben Stiller movie.

[trampus]

What I am trying to do is replicate the G75 groove cycle from a GE/Fanuc (Hardinge T-42SP) to the Okuma OSP-P200L . I am cutting a .034 wide (carbide tool) groove from .570 to .360 dia.(Using GE/Fanuc T-42SP) I lied to the G75 and made it stationary in Z, to peck in and out. I have cut these titanium castings by hand before on a chucker and am aware of the tool pressure, etc. I don't think I need all of these variables in this G73. It is a pain to TRY to understand the programming book at times. Some variables seem to replicate others.

The old program is:
G75R.02;
G75G99X.360Z-.0665P00500Q00000F.0003
It worked so nice I couln't beleive it. Anyway I would like t get i rigt on this new Okuma.
Thanks again.

[zooloader]

G0 X0.600 Z-0.0665
G73 X0.360 Z-0.0665 D0.010 I0.020 F0.0003

From 0.600 rapid to 0.580, then 0.010 pecks(dia) to 0.360

[trampus]

G0 X0.600 Z-0.0665
G73 X0.360 Z-0.0665 D0.010 I0.020 F0.0003

From 0.600 rapid to 0.580, then 0.010 pecks(dia) to 0.360

Thank you.
I guess I don't need all the other variables.It sure is plain and simple. I'll run that. Get back to you.

[trampus]

G0 X0.600 Z-0.0665
G73 X0.360 Z-0.0665 D0.010 I0.020 F0.0003

From 0.600 rapid to 0.580, then 0.010 pecks(dia) to 0.360

Thanks, this works perfect!

:wave:

[DouglasR]

G73 grooving and G74 drilling are two of the most convenient cycles for lathes. The "I" word is rarely used in grooving and the "K" word rarely used in drilling but both have their uses. These cycles are true time savers.

I had a job in my LB15 that had a huge groove between two shoulders. G73 was a lifesaver. I would peck down to the X axis target point, retract and shift to the next cut, all in one line - what would've been 60 lines of code. Then I would just program a finish contouring cut and the part was done!

G74 peck drill was invaluable when drilling long holes with small diameters. I'd peck in about 1/2" then full retract to pull the chips out. Worked like a champ!

[leszek0213]

Thank You Very Much To All for help:cheers: