Re: [CAD_CAM_EDM_DRO] Rigid Tapping--How is this accomplished?

Kim Lux wrote:

>I'm in the same boat as you: considering cutting threads in a mill. I
>haven't done it yet. Here is what I know, with questions about stuff I
>don't understand:
>
>There are 3 or 4 ways to cut threads in a mill:
>
>a) rigid tapping
>b) rigid tapping with a floating tap holder (compression/extension type)
>c) thread milling: single point
>d) tapping head
>e) thread formers instead of taps.
>
>a) Rigid tapping: a tap is held in a solid holder. The spindle has an
>encoder and the Z axis is fed synchronized to the thread pitch of the
>tap, just like the Z axis of a lathe is when single point threading.
>
>The thing I don't understand about rigid tapping is how the software can
>get the spindle to speed up/slow down fast enough such that the Z axis
>stays in perfect synch with the spindle. *Any* misfeed of the Z axis is
>going to cause problems.
>
>

I don't understand the problem here. Generally, the spindle rotation
cannot change
very rapidly, due to motor inertia. On most commercial machines, the Z
axis linear movement can accelerate many times faster than the spindle can
change speed. Remember, on a 40 TPI tap, the Z axis only needs to move one
inch for every 40 spindle revolutions.

>b) Rigid tapping with a floating holder. Here the tap holder is spring
>loaded so that it can compress/extend to accommodate some misfeed of the
>Z axis. A holder with compression/extension lengths of 0.5" could
>accommodate 10 revs of misfeed at 20 TPI.
>
>The thing I don't understand about this setup is how the tap can totally
>cut the thread without breaking. For example, if I am cutting a thread
>by hand, I must advance/reverse the tap 25 times to reach the bottom of
>the hole without breaking the tap. How could a milling machine power
>the tap right to the bottom of the hole without reversing the tap ?
>Won't it break the tap ?
>
>

There are special taps used for machine tapping. For blind holes, you
commonly
use a spiral FLUTE tap, which looks much like a twist drill with
threads. It
brings the curly chips up the flutes just like a drill. I use a CNC
tapping head,
which handles the reversing of the spindle when the quill feed reverses, but
the tap doesn't know the difference. I have tapped several hundred 6-32
and
10-32 holes in minutes with these taps. the tap is just run all the way
in in one
pass, then brought back out.

>c) Thread milling: single point and other...
>
>Thread milling works like helical machining, except that the cutter is a
>single point threading tool fed at a coarse pitch (ie the thread pitch)
>rather than an endmill. In thread milling, the Z axis is fed downward
>at the thread pitch while the X and Y axes do a circular interpolation.
>Note that several passes must be done at various diameters to get to the
>final thread depth.
>
>The caveat of this method is that the tool must fit in the hole and thus
>it is generally only useful for larger holes. Tooling catalogs sell
>special thread mills for doing fairly small holes (ie < 5/16"), but they
>get expensive, ie $200. A thread mill will work for any hole size
>provided the pitch is right. A single point tool will work for any
>thread that you can get it in the hole for.
>
>

I got a single ROW thread milling tool, for about $45. It will do
1nything above
1/4" major diameter. It has 4 teeth with an OD of 1/4". I have milled some
oddball threads in aluminum and aluminum bronze, and they looked BETTER
than tapped threads! it is not as fast as tapping, but for special
threads, and
where it is not practical to mount the part on a lathe for single-point
threading,
it is a great thing.

>It takes special software to do this operation. I've written such a
>routine for TurboCNC but not yet tested it. BTW: the canned cycle for
>helical milling will NOT work because most will break the threading tool
>when they retract, among other problems.
>
>

I have a program that writes the G-code for this. See near the bottom of
the page at http://jelinux.pico-systems.com/gcode.html
I really need to put taper in so you can do pipe threads, too.

>d) Tapping heads.
>
>A tapping head is a device that feeds and reverses a tap into and out of
>a hole until it is tapped. I've never used one. People tell me they
>are tricky to set up. They've got a torque setting. I think they will
>go as deep as they are fed.
>
>
>

I have a PRocunier model 15000 "CNC" tapping head. It has no overload
clutch, otherwise it is similar to the non-CNC units that don't have a
leadscrew.
You program in the spindle RPM and dividing by the thread pitch gives
the Z feedrate. Retraction is at twice the forward feedrate on most models.
I have used it with no trouble, as long as I didn't ram the tap all the way
to the bottom of a blind hole. I have a program to write the G code for
this, too.

>We cut a lot of threads in our work. I want to get automated tapping
>going as soon as possible.
>
>I spoke with a CNC mill owner about tapping and he highly recommended a
>floating tap holder, especially for one off holes as there is no fooling
>around with torque settings as there would be on a tapping head. He
>said that in a production setting he has tapped 1000s of holes without
>breaking a tap. I just can't fathom how one could drive a tap from the
>top to the bottom of the hole without reversing it and without breaking
>it.
>
>

Try the spiral flute taps, you will be amazed.

Jon