[bradlar90]

I have a Sieg IKC4 CNC slant bed lathe, Fanuc Type B I believe. Got an issue where the G76 threading command runs, but for some reason takes the first pass at full depth, and then pulls out and continues with the rest of the passes just cutting air. Does anyone know what could be causing this?

Here's what I'm running, I'm told that the 2-line format is correct for this machine.

G76 P050060 Q0.1 R0.02
G76 X23 Z-20 P1 Q0.2 F2

In this example I'm trying to cut an M25*2 thread, but the first pass is at X23.00 which is full depth. The next pass will then be at something like X23.42, the next at X23.36 and so on until the final pass is back at X23.00.

Can't figure it out, any help would be appreciated.

Cheers

[rcs60]

Here's what I'm running, I'm told that the 2-line format is correct for this machine.

G76 P050060 Q0.1 R0.02
G76 X23 Z-20 P1 Q0.2 F2

you are using dec. points in the first g76 line but the p in the 2nd line has no dec. point

some fanucs 31i's from citizens machinery do not allow dec. points in the P,Q,OR R
as these ae sub micron machines they are 5 place figures 00300=.003 and if not programed this way it does what you are talking about full depth on the first pass and .00001 on the subsequent passes

M3S1=1200
T200(9/16-18 THREAD)
(LAY DOWN 18 TPI INSERT)
G0X.662Z.775T2
G4U.5
G76P010015Q00300R00100
G76X.4938Z2.360P03410Q00900F.05556
G0X.662
G0X.662T0

you will have to change some as you are using metric instead of English
practical machinist does have a good g76 description in there blog

[Superman]

Ps & Qs cannot have decimal point
so

G76 P050060 Q0.1 R0.02
Pxxyyzz xx= # of finish passes,..... yy # of revs before Z depth for pullout,........ zz=plunge-in angle
..........Q is depth of cut in microns,.... R is depth of finishing pass
so try G76 P010029 Q100 R0.02

G76 X23 Z-20 P1 Q0.2 F2
P is radial thread depth in microns,...... Q is depth of 1st cut in microns
so try G76 X23. Z-20. P1000 Q200 F2.

LINK

[sinha_nsit]

P----60 would also work (one-side cutting)