Thread milling - tapered threads

[Jeff_Birt]

I bought a 1/16-27 NPT thread mill for a project. When I went to configure the thread milling parameters for an internal thread I ran into an interesting problem; what value should be used as the major diameter? Since the threads are tapered there is no single major diameter. I read through the section of Machinery's Handbook on pipe threads and found several diameters specified (values for 1/16-27):

Effective Thread, External - 0.28750", This is shown as effective thread length w/approximately two usable but imperfect at crest threads.

Nominal Perfect External Threads - 0.28287", The diameter at the last  'perfect' thread

So, I was not sure which, if either, would be correct. Then I got to wondering if your doing external threads you would want to keep going until the nominal diameter of the pipe (a couple more malformed threads.)

Anyhow, it just got me wondering about the best way to approach thread milling tapered threads and since I did not have a ton of them to do I just tapped them by hand whilst pondering how to set it up properly on the CNC mill.

Any thoughts?

[Bob La Londe]

I would think if you calculated the major diameter of the mill at the surface when its at its maximum depth you will be dead on.  The problem I think will be that the load on the mill will increase as it spirals deeper, and there will be almost no cutting load when you first start. 

[lloydsp]

More to the point, it depends upon how deeply you want the nipple to engage.

A 'standard' Irwin pipe tap won't bottom-out the nipple at the last thread until the entire cutting length of the tap has come flush to the top of the work.  It's designed that way.

YMMV.   But no matter what, you're going to have to play with it a while to get the right engagement and not too much.

LLoyd

[Jeff_Birt]

I don't think this setting should be arbitrary or require fudging, after all what is the point of a standard then?. Since for an internal thread you would not want any 'imperfect' threads I would guess that the: Nominal Perfect External Threads - 0.28287", The diameter at the last  'perfect' thread, would be what was needed. For external threads it seems a bit murkier in my mind.

[lloydsp]

Jeff, it shouldn't be subject to adjustment, but it is; primarily because various brands of nipples vary slightly in o.d.

Certainly, a standard tap IS a standard.

Lloyd

[coolant slinger]

Jeff,
I threadmill a lot of NPT & NPTF threads at my day gig. We make vavles for the natual & LP gas industry.  I don't think Cambam will do a pipe thread. See, the dia. will change with every revolution when milling a pipe thread. I use a free software Advent2008. You can download it from their website.
The machinery handbook calls for the Major diameter to be .3125". I ran it through Advent and it said .302061" dia.
Here is the screen shots and the code for the thread. Note that it is programmed to tool center or part line. You will need to use cutter comp of 1/2 the tool dia. at the small end of the tool or tool tip. I assume you are using a tapered multitooth threadmill. hope this helps.

[Bob La Londe]

Old thread. New thought. 

Is the consensus still that thread milling pipe threads isn't done in CamBam?

My thought is if I can create a taper helical polyline in CAD I could then create an offset of it (not sure cambam can do that), probably also in CAD, with an offset value the radius of the cutter.  With some creative manipulation then it could be scaled in XY (Z wouldn't change) in CamBam to fine tune it. 

How are you guys doing it? 

In the past I have always just used taps and dies for one off or a couple parts, but now I am looking at some short run production parts. 

[Bob La Londe]

I just looked at ViaCad.  I can draw a helix with length, diameter, pitch, and draft angle, so step one seems pretty easy.  Then add some leads to the polyline, and engrave.

[Bob La Londe]

Nope.  Not quite.  ViaCad won't make an offset of a non planar polyline, but it can be drawn with a diameter reduced by diameter of cutter. 

[dh42]

Hello Bob

There is a Tapered.js script that exist (installed with CamBam) that allow to generate tapered path. With using it multiple time and changing the diameter you can generate multiple toolpath as on the picture.

To do the one on the picture, I generate first a path with:

var radius_1 : double = 25;         // Start Radius
var radius_2 : double = 20;         // End Radius

then another with:

var radius_1 : double = 24;         // Start Radius
var radius_2 : double = 19;         // End Radius

var depth_increment : double = 3;   is the pitch

Unfortunately seems that CB V1.0 no longer support JScript, but it works with the 0.98 if you still have it installed.

Maybe someone can convert it to python so it will works on V1.0 64bits ; if nobody can do it, I can try to convert it to a plugin ....

If you don't want the move to center at the bottom, remove the following lines:

// move to center
p.Add(0,0,z);

The script do not take tool diameter in account, so you must give the diameter of the toolpaths, not of the hole.

I have a try with the "profil to helix" plugin, but it compensate for ballnose and we do not get the right toolpath ; if we try with a tool diameter = 0, this do not work.(tool diam must always be > to depth increment)

++
David