re:Re: mill threading

Alan writes:

>Great! So we just "inch" our way into the taper (a series of
>offsets) and repeat them.

The taper (angled line) IS the thread "path" to be followed. As you
say, the thread "unwound". Any approach moves will be "normal" X in
length, rotate to position, and Z (down into material).

If you do complete "turns" of thread, the toolpath in CAD will look
like a wood handsaw blade held vertically (oops, sawtooth wave form:
you're a radio guy<G>). Be sure to code the Z "up"(out of material)
move(s) and the Z down (into material) moves (at each end of the
angled lines). Or as you say, use tool offsets (where each tool is
shorter than the previous one BY the depth of cut you wish to make)

>Or I guess they could be cut in one pass of the length of the
>thread?

Depends on material and cutter. Several passes would be better,
usually. There is a company in the woodworking world called Beall.
They make a router based wood threading tool which uses this sort of
setup(vee-groove tool, plunge in). They sell 60 degree vee-tools. I
think they have carbide. Might not be the best grade for some metals,
but it's a place to start, IMO. Try a local Woodworking specialty
store.

>Sounds like the dovetail cutter might be easier to get into the
>stock. Saw the 14400 correction in your later post. So Y is going
>to be 3.6" * #threads/inch * length of screw.

Yes, cutting with the periphery of most tools is desirable.
Yes. 3.6 inches is the CAD equivalent for steps required (at 8000
SPI) to rotate one revolution. So a one inch long thread, 10TPI, will
be "drawn" as an angled line which goes up(or down)36 inches while
moving across the screen one inch. Then lift the z axis, move back
one inch, re-insert the cutter a little lower, and repeat...

>A ThreadMill? Special endmill?

Yes. Looks like a circular bellows(crossed with a tap). No pitch,
since the helix does that. For production use, it cuts many "threads"
in EACH 360 degree helix. Simple version can be ground from a keyway
cutter. (Dremel makes one. Looks like a SMALL "circular saw" at the
end of a shaft)

>Does the cutter (vee case) feed in 90deg? Seems like on the lathe,
>the compound rest is used to feed in at an angle? I could be
>confused!

Yes. On a lathe, the compound is often set at 29 degrees (for a vee-
thread). This is so the cut is taken on mostly ONE flank of the
thread. Better cutting action. Easier on the tool. Better surface
finish.

You have "live" tooling with the mill setup, so except for the vee-
point mentioned (earlier post), cutting "straight in" is OK.

Glad to help.

Ballendo