[serickson]

I need some help making G76 multi-repeat threading work.
The machine is a Daewo Puma 8HC-3A with Fanuc 15-TF control.
I want to thread 1/8” NPT on brass.
27 Threads Per Inch, thread lead = 0.037037”. Will simplify to .037”
From charts, thread depth = .027”
From charts, the thread length is ~3/8, so I will use .4” to be threaded onto my brass
Major dia at big end from charts is .405
The tool start will be positioned .2” in front of stock, making that a Z0.200” dimension, a Z total travel of .6”.
Extending he slope of standard pipe threads makes the X position at that lead-in to be 0.3675”
Total X diameter change over Z stroke of .600” is: .405 - .3675 = .0375”
In trying to understand the G76 operation, I want a 1st cut depth of .001”, a minimum cut depth of .001”, finish allowance .001”, and 1 finish pass.

Here is the code I have tried:

(THREADING HERE)
G20 G56 G90
G97 G98 M17
M42
G50 S2000
T0606
G00 X1. Z5.0
M03 S60
M08
Z.200
X.3675
G76 P010060 Q10 R10
G76 X.351 Z-0.400 P270 Q10 R-375 F.037
G00 X8. Z10.0 M05
M09
M30
%

Removed stock from chuck, so as to just observe process cutting air.
The above code (with S700 code) results in 10 threading passes, but they didn’t look right.
Changed to S60 so as to observe what’s going on. I monitored the X & Z positions during the threading passes, and X DID NOT CHANGE during the Z movement from +.2 to -.4
And the X values didn’t make sense to me. Below is what I observed for X positions during the 10 passes.

Pass # X @ start X @ end
1 .361 .361
2 .371 .371
3 .381 .381
4 .391 .391
5 .401 .401
6 .411 .411
7 .421 .421
8 .276 .276 <<<<<==== ??
9 .351 .351

Very bizarre results.

Sure need some help with this.

Cheers

[sinha_nsit]

G76 P010060 Q10 R10
G76 X.351 Z-0.400 P270 Q10 R-375 F.037

Many things are parameter dependent. May try the following:
Replace R10 by R0.001
The min DOC must be smaller than the first DOC. Therefore, replace Q10 in the second block by Q20
Replace R-375 by R-0.0375/2 i.e., R-0.01875 (R is a radius value). Use a rounded figure R-0.0188

Also, delete G90 in the first block. I believe, you are using G-code system A.
In inch mode, up to six digits after decimal are allowed for F, irrespective of the increment system being used on the machine, though it is IS-B, mostly.
Therefore, for better accuracy, may use F0.037037

For detailed information about threading (G92, G76, G32 & G34), may refer to this.

[serickson]

Thanks for the response. I will be trying your suggestions tomorrow, but I did come across information in the yellow Fanuc book that has allowed me to successfully make the G76 threading operation work.
From the book: G76 X__ Z__ I K D F__ A__ P__
The actual code that worked for me was:


(G71 MULTI PASS TURNING)
(MAKE STRAIGHT TAPER)
( TO ACCEPT THREADING)
G00 X.55 Z0.2
G71 P200 Q201 U0.01 W0.010 F.007 D0150
N200 G01 X0.380 Z0.0 F.05
X.405 G01 F.007 Z-.400
N201 X.55 Z-0.475
G70 P200 Q201
G00 X.7
M05
M09 G00 X10.0 Z10.

(NEW G76 TEST)
G20 G56 G90
G97 G98 M17
M42
G50 S2000
T0606 S1450
G00 X.45 Z.2 M08
M03
G76 X.351 Z-.4 I-.0187 K.027 D0020 F.037 A60 P1
M05
M09
G00 X8. Z10.
M30


Again, Thanks
Steve

[sinha_nsit]

This is 1-block format.
A machine is set for either 1-block or 2-block formats. Both do not work at the same time.