95 LNC 8 threading help

So I have been learning this machine (95 LNC8 with 5020L) and have had some great success. Now I am trying to get any threading cycle to work and I am having some trouble. I am brand new to cnc lathe and this is my first Okuma. So I have a few things to overcome I know. I am doing .685X40 internal threads. I have the program set up to do 2 passes and a spring pass. Here is my problem. If I run a G32 cycle as generated from Fusion, the machine alarms out with a 450B data word X,Z alarm. In my research I see Okuma wants the X positions on the G32 line. So I added the redundant X positions to the G32 line of code and it runs. I set my work Z offset 1 " away from the part and watch it run. Looks like it rapids down the hole in Z and moves back in a feedrate speed like creating reverse threads. I have no doubt I am doing something wrong here. I then tried to generate a G71 threading cycle to do the same job and the machine alarms out as soon as it gets to the G71 line. Sadly I did not write that alarm message downas this beatdown took its toll today. Here are a few pics of the Code I am working with. Please help me find the holes and let me know what I am doing wrong here. I do know this machine is very picky on the code it will run due to its age and "Okumaness". I am still learning what that is. This is my first attempt to thread anything on it.

First pic is as generated G32 (wont run)
Second pic is G32 with redundant X on G32 line (runs but not correctly)
Third pic is G71 as generated.

I would really like to make the G71 work. I am just unsure if the machine can run it at all or if there is something I need to change thats out of place for this machine.

G32 is for x axis threading
G33 is for longitude threading

G33X.xxxx Zxxxx F= THREAD LEAD
G33X.xxxx

N6
(THREADING BAR)
(THREADS 3/4-48 THREAD)
G0G97M3S1000T0606M8M42
G0X1.100Z.200
G71X.7194Z-.360B60D.006U.002H.0128J48F1
G0X1.00Z.200
M8
G0X15Z2.00
/M01

X=X
Z=Z
B= IN FEED ANGLE
D=1ST DEPTH OF CUT IN EXPRESSED IN DIAMETER
U= FINISHING ALLOWANCE IN DIAMETER
H= THREAD HEIGHT IN DIA.
J= THREAD PITCH
F=1 (ENGLISH ) AS THIS TAKES F/J FOR FEED RATE

Thanks a lot for the help. I wrote the threading cycle line with G71 a few different ways and I never got it to work. I ended up trying the G33 cycle. What finally worked was G33 with adding the redundant X position to the line of code.

Here is my final program for .685x40 threads. (.665 minor .685 major) ( Done in three passes and a spring pass )
Tool is a Micro 100 (2001000 thread tool)

G50 S2000
G0 X400.
G0 Y400.

T040404
M8
G95
G97 S300 M3 M41
G0 X0.665 Z0.1969
G0 Z0.04
X0.6717
G33 X0.6717 Z-0.59 F0.025
G0 X0.650
Z.04
X0.6783
G33 X0.6783 Z-0.59 F0.025
G0 X0.650
Z.04
X0.685
G33 X0.685 Z-0.059 F0.025
G0 X0.0650
Z0.04
X0.685
G33 X0.685 Z-0.059 F0.025
G0 X0.650
Z0.1969

M9
G90 G0 X400. Z400.
M2
%

i have gotten a ton of help from this community and I really appreciate it. You could pretty much thread anything with this format. I now know that. I hope this helps someone that struggled with this as I did.

hy :) please check attached threading section from the manual

i also have re-writen your code

for smooth finish, use spring pases combined with re-cutting the crest ( using the tool before the thread ) and the chamfers ( towards the root diameter ); operations type & order, and number of repetetions, may vary, depending on threading insert and others

g33 is more powerfull than g71, since it allows better control, but coding it is a bit more demanding

i have used g33 for years, but lately i switched to g34, in order to better manage vanished treads and repositioning motions

is possible to eliminate one turret index, by cutting the chamfer also with the threading insert, using one extra offset, ... and there are others tricks as well / kindly :)

Code:

---



    G50 S2000
    G00 X400 z400


    T040404 G97 S300 M03 M41 M08
        X0.665  Z 0.04
    G33 X0.6717 Z-0.59 F0.025 G95
        X0.6783
        X0.685
        X0.685


    G00 X400 Z400 M09 T0400


M02

---