What's new
What's new

3.5" NPT G76 Cycle

Changed


G01 X3.7286 Z.2 F.05 M08
G76 P040055 Q0100 R0005
G76 X3.8036 Z-1.0039 P1000 Q0030 R-.0376 F.125
I'd change to this:

G01 X4.08 Z.2 F.05 M08
G76 P040055 Q0030 R0005
G76 X3.848 Z-1.7 P964 Q0150 R-593 F.125

You should start above the major at the end of the thread
Your min DOC was .01 and the first DOC was .003
The overall length of a 3 1/2-8NPT is 1.6837, hence the change to Z-1.7
The thread height is .0964
 
Now I noticed that the Z value start before each pass gets closer to the face of the part. Is that normal. Never noticed it before.
 
Now I noticed that the Z value start before each pass gets closer to the face of the part. Is that normal. Never noticed it before.
Yes. That's because you have a Tool Tip included angle specified in the "P" address of the 1st G76 Block. By specifying a Tool Tip Included Angle, most, or all, depending on the angle specified v the actual included angle of the Thread Form, will be made by the Leading Edge of the insert. The control makes this happen by shifting the Z Start Position of the Tool. As I've mentioned in this Thread before, this shifting of the Z Start also introduces a very slight error in the Taper specified by "R" in the 2nd G76 Block.

You've specified a 55-degree Tool Tip Included angle, therefore, most of the cutting will be carried out by the Leading Edge of the insert and a small amount by the Trailing Edge of the insert when cutting a NPT Thread.



Regards,

Bill
 
Last edited:
Yes. That's because you have a Tool Tip included angle specified in the "P" address of the 1st G76 Block. By specifying a Tool Tip Included Angle, most, or all, depending on the angle specified v the actual included angle of the Thread Form, will be made by the Leading Edge of the insert. The control makes this happen by shifting the Z Start Position of the Tool. As I've mentioned in this Thread before, this shifting of the Z Start also introduces a very slight error in the Taper specified by "R" in the 2nd G76 Block.

You've specified a 55-degree Tool Tip Included angle, therefore, most of the cutting will be carried out by the Leading Edge of the insert and a small amount by the Trailing Edge of the insert when cutting a NPT Thread.



Regards,

Bill
AH OK. Say I change that to 60 it would cut completely centered?
 
AH OK. Say I change that to 60 it would cut completely centered?
If you specify a 60 degree Tool Tip included angle, which is the actual angle of the Tool Tip for a NPT Thread, then all of the cutting will be made by the leading edge of the insert. To have both the Leading and Trailing edge of the insert cut equally, the angle specified would have to be Zero.

Regards,
Bill
 
Trying to learn just by trial-and-error and asking others, without reading any book/manual, may seem to be a smart short-cut, but one actually never learns beyond a certain level. This is fine for button-pushers, but not good for somebody serious about his career.
 
Trying to learn just by trial-and-error and asking others, without reading any book/manual, may seem to be a smart short-cut, but one actually never learns beyond a certain level. This is fine for button-pushers, but not good for somebody serious about his career.
Again you didnt link anything to me. And I asked you to send me a link in PM or here. And again I am serious, but im typically not programming anything like this. And I have books on programming just in storage as im currently living in a small apartment with not much room. So again I will be happy to look but again no linky.....
 

May read any book/manual. The above is my write-up (Post # 150), based on Fanuc manual. Download is free for two more days.

My advise is, purchase SINHA's Handbook of Fanuc CNC Lathe for $2.99 only. It is a 400-page book (print length). Read it for a couple of days. If you do not like it, return it for full refund.
By the way, there has not been a single return for this book, so far.
It contains the updated versions of all my short books, including the above book.
Link for kindle version: https://www.amazon.com/dp/B0CR9DXP4T/ ($2.99)
Link for paperback: https://www.amazon.com/dp/B0CR2SDL1F ($13)
Paperback is also returnable within 30 days of receipt.
 
Last edited:
I do not know the dimensions you're trying to hit as I have not drawn up the thread with the proper start and end point diameters, but if you have either a decent solid modeler with the ability to properly model a 3.5-8 NPT, then you can get your dimensions from there.
As far as the G76 cycle itself:

G00 X(start.minor.diameter) Z(start.of.thread)
G76 P(ffccaa) Q(depth.of.cuts) R(fin.allowance)
G76 X(end.minor.diameter) Z(end.of.thread) R(taper) P(thread.height) Q(first.pass.DOC) F(feedrate)

ff= # of finish cuts
cc= chamfer size (0)
aa= thread angle (60)
end.of.thread= The Z-length where you program the path to.
end.minor.diameter= diameter @ end.of.thread (from CAD drawing)
start.of.thread= The safe distance in front of the part where you start each threading pass from
start.minor.diameter= diameter @ start.of.thread (from CAD drawing )
taper= (start.minor.diameter - end.minor.diameter ) - for NPT this means R is negative for OD threads, R is positive for ID threads!!!
thread.height= from CAD drawing

For the numbers, the best I can do is this: 3 1/2-8 NPT - Courtesy of ME Thread Pal

View attachment 424044
So I was looking into purchasing thread pal but it seems as they are no longer taking payments or they no longer sell the software.
 
So I was looking into purchasing thread pal but it seems as they are no longer taking payments or they no longer sell the software.

Yeah, that's a pity.
Here is a thread that talks about it extensively, perhaps there might be some resolution to it sometime in the future.
 
Yeah, that's a pity.
Here is a thread that talks about it extensively, perhaps there might be some resolution to it sometime in the future.
So I found some information on the thread pal creator. Believe his name was Mike. Seems like he was in his late 70s and there is some talk that people believe he passed away. Found out from some dudes on Reddit who also experienced the same issues trying to buy thread pal
 








 
Back
Top