[RussMachine]

I tried using the Threadmilling Wizard supplied with Mach3, but it doesn't have a Wizard for NPT Threads, only straight threads.
GGRRRRRR... :devious:
I need to make a part that's 2" -11.5 NPT, external threads,
My lathe doesn't have a taper attachment either, so I'll be threadmiilling it on the TORMACH.
If I can't find a Wizard, I'll be hand-coding it (boooo).
Anyone have an O.D. 2" NPT program already written?
Any online wizards available?
HELP!

[MichaelHenry]

I used an NPT thread mill to tap an NPT female thread in PVC a few years ago and generated the attached tap file. I don't remember for sure now, but the hole was probably 1-1/2-in NPT. I probably used far more ops than necessary and am including just the thread mill segment here but perhaps this will get you started.

Mike

[GLCarlson]

Russ,

Go here:
Single Point Threadmilling Tutorial - YouTube
get the advent2008 software referenced. If you can't find it, pm me, I have copies.
This is easily the best instruction on threadmilling I've ever seen. The Advent code has everything-NPT, metric, inside, outside, etc.
Generates g code for Tormach just fine. It's a bit clunky to use until you work with it- biggest hangup is choosing the right cutter.
My first try ran perfectly- despite a whole lot of trepidation.

[RussMachine]

Thanks for the advise guys.
The problem I have is calculating the 1°47' angle while threadmilling down.
A straight thread is no problem, just M02 circle-mill and ramp down in Z whatever the pitch is.
With the NPT thread, I also need to add the 1°47' taper with every Z move.
I couldn't find any descent Wizards online.
The only good one I found couldn't switch from Metric to imperial.

[SCzEngrgGroup]

For a tapered thread, you have to specify short arc segments, with the specified radius and arc center slightly offset from the actual centerline of the part, so you end up with a piece-wise approximation of the desired thread profile where the start and end point of each arc are exactly on-target, and the radius is the average or the starting and ending radius for the "ideal" arc covering that distance. How long (or short) those arc segments can be is a purely function of the accuracy you're after. I would expect for any reasonable application, 90 degree segments would probably be more than adequate. You can also do it as a series of very short linear segments. Done properly, that can give you better overall accuracy, but at the expense of FAR more lines of code.

Regards,
Ray L.

[RussMachine]

Ray, how would 180° segments fare?
I'm milling a 2" External NPT - 11.5 Pitch
1 ÷ 11.5 = .08695 per full thread.
So, a 180° segment would be .043475 Pitch and angled out at 1°47' (1.7899)
............
SOOOOOOO..... in conclusion (after some fancy Trigonometry)
For every 180° arc, I should move down in Z .043475, and move my radius out .00135.
Continuing the downs and outs until I reach my final depth.

[SCzEngrgGroup]

That should work fine, if you generate the code carefully.. The only thing you need to be careful about is accumulating errors correctly when generating the code. If you use 0.00135 as the increment for every arc segment, by the time you've done 5-10 threads, you may have enough error, due to rounding, to be a problem. Either calculate the exact offset for each arc endpoint, or keep track of the error in each segment, and correct for it as you go, by tracking the accumulated error.

Regards,
Ray L.

[acannell]

or you can get a tapered thread mill..

I got this 11.5tpi NPT thread mill on ebay for $20 I think and it has a taper..I'm saving it for when i need to make some huge NPT on my 2hp mill

im not completely sure if the taper this has means it can just be spun in a straight spiral or not..

[SCzEngrgGroup]

No, you still must make a decreasing-radius helical move.

Regards,
Ray L.

[acannell]

No, you still must make a decreasing-radius helical move.

Regards,
Ray L.

I wonder what the point of the taper is then?

OP: you could have someone with a CAM software that can generate the right G code send you an NC file and then you could use it..should be pretty easy..plus it would be interesting to see how it does it

[SCzEngrgGroup]

I wonder what the point of the taper is then?

The point is you can cut the threads very quickly, because you only have to go around once, rather than 10-15 times. But the required motion is exactly the same as is required for a single turn with a single-point threadmill.

Regards,
Ray L.

[SCzEngrgGroup]

BTW - That will be good only for pipe between 1" and 2". All other NPT threads are a different pitch.

Regards,
Ray L.

[acannell]

BTW - That will be good only for pipe between 1" and 2". All other NPT threads are a different pitch.

Regards,
Ray L.

Thanks! Can I drill a hole with it? What other things cant I do with it?

[RussMachine]

No, you can't drill with it.
It's only good for side-cutting.
The taper is on that style of threadmill so you can cut the thread in only one helical pass.
..
With a single-point threadmill ( 60° included cutter, one tooth), you would need to helical cut EVERY tooth of the thread.
That's my dilemma, from my original post.
..
If I had your style of threadmill, I wouldn't need to calculate the 1.7899° angle per revolution.

[acannell]

No, you can't drill with it.
It's only good for side-cutting.
The taper is on that style of threadmill so you can cut the thread in only one helical pass.
..
With a single-point threadmill ( 60° included cutter, one tooth), you would need to helical cut EVERY tooth of the thread.
That's my dilemma, from my original post.
..
If I had your style of threadmill, I wouldn't need to calculate the 1.7899° angle per revolution.

are you still trying to figure it out or are you going with the segmented toolpath you mentioned below

[SCzEngrgGroup]

If I had your style of threadmill, I wouldn't need to calculate the 1.7899° angle per revolution.

That's not right. The motion to use a multi-point threadmill is exactly the same as required for a single turn of thread using a single-point threadmill. If you do just a pure helical move, you'll end up with a small "step" at the start/end point of the cutting move. With a tapered pipe thread, that could become the source of a leak.

Regards,
Ray L.

[hoss2006]

Russ,
Check out Machinist Toolbox, Machinist Toolbox
One of the many valuable features is Advanced Threadmilling, it will generate the code like the wizards, you can pick single point threadmilling, also NPT threads from the menu and it will input the numbers for the size you want.
The trial is for 15 days and will output the code for this to see if it works for you.
Well worth the $100 though.
Hoss

[acannell]

you could also use excel to generate the GCODE..Ive done that before for making a spherical 3 axis toolpath

[RussMachine]

Ray, If you ramp in and ramp out of the cut while still moving in Z, it wouldn't leave a step, would it?
...
Thanks for the Link, HOSS. I saved the programs to my PC and I'll be experimenting with them.

[RussMachine]

SUCCESS!!!!
Here's the finished part.
OD is 2" NPT, inside thread is a screwball Medical fitting thread, 1-1/16"-16.
I was able to threadmill both sides.
I used the NPT Thread mill Wizard from Machinist Toolbox (Thanks for the link HOSS).
I also had to put ALOT of cutter Comp on it. ( +.140) Glad I started big!
I wonder if I should charge the Hospital $20,000 , since one aspirin in the Emergency Room costs $500.
.