What's new
What's new

Any tips on single point NPT ID and OD threads

Whuh! That's a little broad question.
You're interested in gaging or setting up and making the threads?

For starters maybe, the taper amount is measured from the end of the thread to the beginning of the thread. This means an OD NPT will have a negative taper, while the ID NPT will have a positive taper amount.

That was my WTF dilemma the first time.

But as I've said, may want to narrow your question a little.
 
Maybe not as straight forward as standard threads, but it's still just a thread.
I always turn/bore the taper to 3/4"/foot, never just use a drill.
Then I draw the start and end points of the minor in CAD, get the radial difference for the taper amount to plunk in the G76 cycle.
REMEMBER! The start and end points if your TOOL that's important.
IOW if you start threading .1 from the face and thread .2 beyond the L3 length, you HAFTA! use those X values in the cycle!!!
 
Seymour,

"Then I draw the start and end points of the minor in CAD, get the radial difference for the taper amount to plunk in the G76 cycle."

Should that not always be the same, the taper amount?

"REMEMBER! The start and end points if your TOOL that's important."

I assume you meant "of" your tool.

"IOW if you start threading .1 from the face and thread .2 beyond the L3 length, you HAFTA! use those X values in the cycle!!!"

Doesn't the G76 start away from the start point with a bit of dwell anyway?
 
Seymour,

A:
Should that not always be the same, the taper amount?

B:
I assume you meant "of" your tool.


C:
Doesn't the G76 start away from the start point with a bit of dwell anyway?


A: Nope!!! The taper amount is dependent on where you start from and where you end. The actual taper is the radial difference between those, the ACTUAL start X and the ACTUAL finish X points.

B: Yup, thick finger syndrome and dyslexia is a common occurrence here.

C: Nope, the G76 cycle starts from where you positioned the tool JUST BEFORE the cycle is invoked.
 
THAT's why TAPS and Dies are made


Gary, care to see some drawings where the notes explicitly require SINGLE POINT THREADING for the ports?
Threadmill is allowed, tap and dies are not.
Similarly, you just ain't gonna make an acceptable NPT thread for aircraft standards with a die. Tap, maybe, but certainly not a die.
 
I have the gauges, well at least a L-1 OD and L-1 and L-3 ID.

Small stuff, 1/8 and 1/4.

Any been there done thats would be appreciated.

You doing this on a lathe, since your talking about single pointing. There is a process for doing it in a mill, with the tool following the lead and the taper. Never done it,looks like a tremendous PIA, only practical on ginormous threads, IMO.
So that leaves us with the subject at hand. I was going to suggest thread milling, but your in a lathe obviously, and not one with live tooling?
What Seymour is trying to communicate is for you to be sure you account for the full Z travel, including your amount that you start from in front of the thread, plus the amount you run past the thread. Programming for only the taper amount(3/4/inch), then moving say .2 longer than the part, in order to start and finish in the clear, would give you an incorrect taper. Bad part is, depending on how much you missed it, you might not notice it with your gauging. Can you say "scrap"?
I like to start my G76 about .1 in front of the part, in order for the machine to have plenty of room to get the lead worked out. Old habit really, from doing this on a manual with a taper attachment. CNC with it's ball screws and encoder can start much closer. How far you run out the ack of the thread is up to you and whether there's a shoulder back there. But with the sizes your talking about, tool length is gonna have a lot to do with it also.
I agree with the idea of tapering the raw hole before you thread it. Sidesteps a lot of problems, again with that tiny tool, you need all the help you can get.
In your G76 cycle, assuming you use the two line version ,the taper is in the R dimension, in the second line. Expressed in a radius. This is where you program the taper in your threads. Just remember to trig out how much taper you need for the full amount of Z travel your tool will encounter, whether it's actually making chips the whole way or not. As you can probably tell, I program this stuff in longhand, with no CAM. We use what we have.
 
You don't need to "trig" anything out. The taper amount is .75 per foot or .0625 per inch, so if you are traveling 2" along the Z axis than your taper amount is going to be .125 radially. If you are travelling .1" plus 2 " because you are starting .1 in front of the part than the taper amount would be .1313 :):cheers:

Robert
 
Hi,

Here is what we ended up with. Thanks for the help and please comment.

(1/8-27 NPT FITTING)

(RUN TOOL 1 TO SET STOCK)
T101
G54
G00 X0.2
G00 Z0.04
M00

M08

(END FACE)
T101
G54
G50 S2000
G96 S250 M03
G00 Z0.2
G00 X0.6
G00 Z0.04
G72 P401 Q402 U0 W0 D0.01 F0.002
N401 G00 Z0.
G01 X0.6
N402 G01 X-0.01
Z0.05
G00 X0.6
M01

(OD TURN)
T101
G54
G50 S2500
G96 S250 M03
G00 X0.6
G00 Z0.
G71 P201 Q202 U0.001 W0.001 D0.01 F0.003
N201 G01 X0. F0.002
G01 Z0.
G01 X0.329
G01 X0.39 Z-0.03
G01 X0.408 Z-0.32
G01 X0.408 Z-0.405
G01 X0.55
G40
G01 X0.6
N202

G42 (TNC RIGHT ON)
G70 P201 Q202 (FINISH PASS)
G00 Z1.

(OD THREAD)
T202
G54
G97 S500 M03
G00 X0.475
Z0.
G04 P1.
M08
M23
G76 X0.3314 Z-0.32 K0.03 I-0.01 D0.002 F0.037
G00 X0.475 Z0.1
G00 X0.6
G00 Z1.
M01

(OD CLEANUP)
T101
G54
G50 S2500
G96 S250 M03
G00 X0.6
G00 Z0.
G42 (TNC RIGHT ON)
G70 P201 Q202 (FINISH PASS)

G00 Z1.
(OD THREAD CLEAN)
T202
G54
G97 S500 M03
G00 X0.475
Z0.
G04 P1.
M08
M23
G76 X0.3314 Z-0.32 K0.002 I-0.01 D0.0005 F0.037
G00 X0.475 Z0.4
G00 X0.6
G00 Z1.
M01

M09
G00 X0.6
G00 Z3.
M30
 
Seymour, Yes I was thinking the same, but with the chamfer it seemed to be just fine.

Is that not a good idea and for what reason?

To do it with a lead in, it will require just some more CAD work.
 
Seymour, Yes I was thinking the same, but with the chamfer it seemed to be just fine.

Is that not a good idea and for what reason?

To do it with a lead in, it will require just some more CAD work.

No, It will take no more CAD work, just move the Z start to Z.2 in both Thread cycles.

If you use the cad for this you are making it to hard.

The reason is to give the machine time to become in sync with itself, the importance increases as the rpm and coarseness of the thread increase. Relates to the machines ability to follow the same path each time and it removes thread lead error.

Jeff
 
No, It will take no more CAD work just move the Z start to Z.2 in both Thread cycles.

If you use the cad for this you are making it to hard.

Jeff


DEAD WRONG!!!!

Moving the Z in the + direction WILL IN FACT change the taper amount!!!
Remember, the taper amount is the actual radial distance from the end X dimension. If you start .2 away from the part while keeping the same taper ( I ) amount, you will have a shallower ( less than 3/4/foot) taper.

Laminar

It really depends on your control. Looks like you're using a single line G76, which may mean a Haas machine. In my early days not knowing any better, I did start at Z0 and have never actually blown a thread.
On the Mori with a '08 vintage Oi-Tc control however, the manual explicitly says to start at a sufficient distance away from the part to allow the spindle speed settling and the feedrate too synchronize with it. It states to start no less than 1 pitch distance away.
 








 
Back
Top