[norfolker]

Hi
Tried this in the Mori forum also,


We've just got an old Mori seiki SL25 MC with an MF T4 control, I've heard its the same as the fanuc OTC control, although we've no manual for either.

Trying to cut a thread using G76, I'm used to this canned cycle with other versions of fanuc
The trouble is, its only doing 2 passes.

Here is my program:

N03(M42 X 4.5)
G28U0
G28W0
T0303(EXT THREAD 4.5P)
G18M46
M8
G97S600M3
G00G99Z5.
X43.
G76P020060Q100R0.05
G76X36.536Z-10.P2732Q400F4.5
G00X50.
G28U0M9
G28W0
M5
M01


I tried changing the R value to an integer (R500) as per an OT manual I have, but then it wants to move miles towards the tailstock in Z for some reason.

also tried changing the Q values to decimals, but it alarmed out.

also tried the following single line code, but it alarmed out:

G76 X36.536 Z-10. I0 K2.732 D250 F4.5 A60


Hoping someone can help

Thanks

Dave

[rcs60]

try to put a leading 0 in front of the Q's it maybe the the control sees this as 1mm minimum cut on the first q and on the second q as 4 mm first cut

G76P020060Q0100R005
G76X36.536Z-10.P2732Q0400F4.5

[norfolker]

Thank you, will try it when i get back.

[sinha_nsit]

The program is correct for a Fanuc. Your control is different. Does it use increment system B? May try Q10 and Q40, if nothing works.

[Superman]

The problem is in the 1st G76 line on the P parameter
Paabbcc
aa = number of finish passes
bb ..... I think it is the end of thread chamfering ie pullout of cut
cc = flank approach angle

You have a 60° side angle, on a 4.5mm pitch thread, the side angle is 30°
- the manual says that only certain values can be used ie 0, 29, 30, 45, 60 ( I think there is a couple more )
- suggest you use P010029, as the infeed cut is down the side of the insert, the 1 degree difference allows for a slight cleanup from the previous passes

if cc = 00, then the threading tool is going to plunge at each pass depth ie cuts on the front & back of the vee insert, it can add extra pressure on the point, & tear the threads

so a 60° infeed makes for a very shallow, but wide thread


the P & Q addresses are the only ones that do not use a decimal point

1st line the R is the finish pass depth
2nd line .... G76X36.536Z-10.P2732Q0400F4.5
X= finish diameter, P=depth of thread Q=depth of 1st pass ........so to work backwards....starting OD is X + ((P + P) /1000) ......OD=36.536+(5464/1000) = 42.000

The G32 / G92 are single shot thread passes, you'd have to string multiple line together to get it to the finish thread size

[norfolker]

Thanks for your suggestions, will try them out.
Can anyone suggest a g92 or g32 threading example that might work if the g76 fails?

[sinha_nsit]

If G76 is available, G32 and G92 should not be used.
You must learn how to use G76 on your control. If manual is not available, trial and error is the way.

[norfolker]

Think I finally sorted it, tried many variations of the G76 cycle but it wouldnt do more than 3 passes. Then I found an OT-C manual online for an Emco lathe which stated G78 as the threading cycle. I swapped G76 for G78 on the 2 lines & it worked!