OK, so I have a CNC mill, in which I know the spindle speed only
approximately.

Can I, realistically, use it for threading through holes, perhaps with
tapping head?

i

Ignoramus8473 wrote:
OK, so I have a CNC mill, in which I know the spindle speed only
approximately.

Can I, realistically, use it for threading through holes, perhaps with
tapping head?

Yes, if you have a Procunier or TapMatic head, it has a forward clutch
that engages when forward pressure is applied on the tap. So, what you
need to make sure of is that the spindle rotation stays ahead of the Z
feed. In that case, the clutch will slip a little here and there to
keep the tap synced with the thread. If the spindle is too slow, it
will mash the tap through the hole, leaving horribly mauled threads. I
had the belt in the wrong step once and did this. So, the spindle speed
should be a little higher than the mathematically calculated value for
the Z feed, or the Z feed should be set a little slower than the spindle
RPM would suggest.

I have a program hidden on my web site to do this,
http://pico-systems.com/recttap.c so you can see what the code looks like.
My Procunier head doubles the spindle RPM in reverse.

on

On 2010-07-25, Jon Elson wrote:
Ignoramus8473 wrote:
OK, so I have a CNC mill, in which I know the spindle speed only
approximately.

Can I, realistically, use it for threading through holes, perhaps with
tapping head?

Yes, if you have a Procunier or TapMatic head, it has a forward clutch
that engages when forward pressure is applied on the tap. So, what you
need to make sure of is that the spindle rotation stays ahead of the Z
feed. In that case, the clutch will slip a little here and there to
keep the tap synced with the thread. If the spindle is too slow, it
will mash the tap through the hole, leaving horribly mauled threads. I
had the belt in the wrong step once and did this. So, the spindle speed
should be a little higher than the mathematically calculated value for
the Z feed, or the Z feed should be set a little slower than the spindle
RPM would suggest.

I have a program hidden on my web site to do this,
http://pico-systems.com/recttap.c so you can see what the code looks like.
My Procunier head doubles the spindle RPM in reverse.

thanks Jon. Great prog. I am already deeply in to writing G code
scripts. I am thinking of providing a website that would generate G codes.

I actually have a tachometer thingy, if I can find a way
attach it the spindle, I could know the speed more precisely. It
counts rotations.

i

Ignoramus8473 fired this volley in
:

I actually have a tachometer thingy, if I can find a way
attach it the spindle, I could know the speed more precisely. It
counts rotations.

Three phase spindle, Iggy? Thre's something there to count. Unless you're
overloading it, the motor should not slip.

LLoyd

I'm not sure if it's practical but you could use a thread mill and a helical
interpolation. Thread mills might be too expensive but it's interesting
anyway!

RogerN


"Ignoramus8473" wrote in message
...
OK, so I have a CNC mill, in which I know the spindle speed only
approximately.

Can I, realistically, use it for threading through holes, perhaps with
tapping head?

i

On 2010-07-25, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
Ignoramus8473 fired this volley in
:

I actually have a tachometer thingy, if I can find a way
attach it the spindle, I could know the speed more precisely. It
counts rotations.

Three phase spindle, Iggy? Thre's something there to count. Unless you're
overloading it, the motor should not slip.

Three phase spindle, the motor always slips and the pulley ratio is
only guessable.

i

Lloyd E. Sponenburgh wrote:
Three phase spindle, Iggy? Thre's something there to count. Unless you're
overloading it, the motor should not slip.


He's got a Bridgeport vari-speed head, it has a dial that shows
approximate spindle speed.
The question was, is that speed dial accurate enough for power tapping
with a tapping head.
Well, probably, as the spindle speed doesn't have to be very accurate,
as long as it is a bit faster than the spindle/Z feed sync requires. If
the spindle spins fast enough, the tapping head clutches slip a little,
and everything is cool. The tap, itself, keeps everything in sync. If
the spindle speed is too LOW, then you get a real mess. That's one of
those "don't ask how I know this" moments.

Jon

RogerN wrote:
I'm not sure if it's practical but you could use a thread mill and a helical
interpolation. Thread mills might be too expensive but it's interesting
anyway!

Multi-row thread mills are REALLY expensive, well over $100 each, and
they only do a single thread pitch. Single-row thread mills can do a
wide range of pitches, and work like some kind of magic, but they are
slow. If you needed to do something like camera threads on the mill,
they'd be great.

But, a CNC mill and a tapping head works quite well, without fancy
spindle sync or precise spindle speed control. The CNC control feeds
the tap into the work at approximately the right feed to match the
approximate spindle speed divided by the thread pitch. Feed a little
slower to let the clutches in the tapping head adjust the rotation. The
CNC control handles the feed depth. When it backs out, the tapping head
reverses the spindle to pull the tap out. If these things work with a
drill press, they can definitely work on a CNC mill.

I have tapped thousands of holes with a Procunier "CNC" model 15000
tapping head. Any tapping head for manual drill-press use should work.
I also did a lot of work using combined drill-taps with the Procunier.
I have just retired it as I figured out how to do rigid tapping on my
CNC Bridgeport.

Jon

"Ignoramus8473" wrote in message
...
OK, so I have a CNC mill, in which I know the spindle speed only
approximately.

Can I, realistically, use it for threading through holes, perhaps with
tapping head?

i

The tapping head is one option.
We used some tapping attachment years ago, I forget what they were, but just
a tool holder with some slip joint in it. Run the feed slightly under the
calculated feed/speed rate, and reverse the spindle and back out the feed at
teh same time. Not sure if it would work in your situation. My bet is you
will be able to find a Tapmatic head cheap enough with your scrounging
abilities.
Greg

On Sat, 24 Jul 2010 20:19:00 -0500, the renowned Ignoramus8473
wrote:

On 2010-07-25, Jon Elson wrote:
Ignoramus8473 wrote:
OK, so I have a CNC mill, in which I know the spindle speed only
approximately.

Can I, realistically, use it for threading through holes, perhaps with
tapping head?

Yes, if you have a Procunier or TapMatic head, it has a forward clutch
that engages when forward pressure is applied on the tap. So, what you
need to make sure of is that the spindle rotation stays ahead of the Z
feed. In that case, the clutch will slip a little here and there to
keep the tap synced with the thread. If the spindle is too slow, it
will mash the tap through the hole, leaving horribly mauled threads. I
had the belt in the wrong step once and did this. So, the spindle speed
should be a little higher than the mathematically calculated value for
the Z feed, or the Z feed should be set a little slower than the spindle
RPM would suggest.

I have a program hidden on my web site to do this,
http://pico-systems.com/recttap.c so you can see what the code looks like.
My Procunier head doubles the spindle RPM in reverse.

thanks Jon. Great prog. I am already deeply in to writing G code
scripts. I am thinking of providing a website that would generate G codes.

Here's a very simple one I ran across recently:

http://eng-serve.com/cnc/excellon_gcode.html

Excellon is the standard for PCB drilling files.

I actually have a tachometer thingy, if I can find a way
attach it the spindle, I could know the speed more precisely. It
counts rotations.

i


Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com

On Sat, 24 Jul 2010 22:24:45 -0500, "Greg O"
wrote:


"Ignoramus8473" wrote in message
m...
OK, so I have a CNC mill, in which I know the spindle speed only
approximately.

Can I, realistically, use it for threading through holes, perhaps with
tapping head?

i

The tapping head is one option.
We used some tapping attachment years ago, I forget what they were, but just
a tool holder with some slip joint in it. Run the feed slightly under the
calculated feed/speed rate, and reverse the spindle and back out the feed at
teh same time. Not sure if it would work in your situation. My bet is you
will be able to find a Tapmatic head cheap enough with your scrounging
abilities.
Greg

Floating tapping "attachments" can be made very easily now that he has
the mill.

Simply machine a slot down a couple inches down the side of a piece of
1" bar, except for the last 3/8" inch, drill a 9/16" hole in the end and
a couple inches into the bar..matching the length of the slot..and
insert a 9/16 bar into the hole. Drill and tap for a socket head cap
screw..and you now have a sliding bar inside a tool holder. Now you can
make up a bunch of similar 9/16 bars..all with the proper hole and a set
screw for each size tap you are going to be using over time.

Id hook a spring to the socket head cap screw and to the 1" body..and
voila...you have a floating, spring loaded tap holder.

Feed in at 75% of your tap lead and the tap will go in, pulling itself
down the slot a smidge faster than your spindle feed rate, and when you
reverse..and pull out..it comes out of the hole faster than you are
retracting. Voila!

Same thing works just hunky dory on lathes as well. I made up a few of
them that I can stick in the mill or the lathe.

I made mine with 3/4 body and 1/2" tap holder rods.. shrug


Its a good first project. If you have a collet tap holder..simply make
the body big enough to hold your collet bar and drill and tap a hole in
the collet tap holder to run in the slot.

Gunner

One could not be a successful Leftwinger without realizing that,
in contrast to the popular conception supported by newspapers
and mothers of Leftwingers, a goodly number of Leftwingers are
not only narrow-minded and dull, but also just stupid.
Gunner Asch

On 2010-07-25, Ignoramus8473 wrote:

[ ... ]

I actually have a tachometer thingy, if I can find a way
attach it the spindle, I could know the speed more precisely. It
counts rotations.

Hmm ... some mechanical tachometers which I have include a
rubber-tired wheel which has a circumference of either 1/2 foot or 1
foot (thus diameters of 0.3.8197" or 1.9099") to reed in FPM or FPM*2.

If you have a surface on the spindle which is cylindrical and
accessible, you can measure the diameter, and calculate the expected FPM
for a given RPM -- then tune for that.

Or -- find a way to mount a magnet biased pickup coil near the
bull gear teeth and count the pulses as the teeth pass by. Of course,
you need to know the number of teeth, but then you can make something
which will convert this into a quite accurate RPM. (Higher speeds don't
need as many sensor points to give speed fairly quickly, but for very
slow speeds, the large number of teeth will give faster readings.

Enjoy,
DoN.

--
Remove oil spill source from e-mail
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

On 2010-07-26, DoN. Nichols wrote:
On 2010-07-25, Ignoramus8473 wrote:

[ ... ]

I actually have a tachometer thingy, if I can find a way
attach it the spindle, I could know the speed more precisely. It
counts rotations.

Hmm ... some mechanical tachometers which I have include a
rubber-tired wheel which has a circumference of either 1/2 foot or 1
foot (thus diameters of 0.3.8197" or 1.9099") to reed in FPM or FPM*2.

It is an electronic tachometer, I think that it counts some kinds of
pulses per second.

If you have a surface on the spindle which is cylindrical and
accessible, you can measure the diameter, and calculate the expected FPM
for a given RPM -- then tune for that.

Or -- find a way to mount a magnet biased pickup coil near the
bull gear teeth and count the pulses as the teeth pass by. Of course,
you need to know the number of teeth, but then you can make something
which will convert this into a quite accurate RPM. (Higher speeds don't
need as many sensor points to give speed fairly quickly, but for very
slow speeds, the large number of teeth will give faster readings.

Don, you made me look, I have made a very interesting discovery that I
will post in a separate thread. (look for one about "What is no top of
the mill head")

i