Rigid Tapping

BigJohnT wrote:

I finally have a VMC that is capable of rigid tapping. At this time it is not running EMC but at the first hiccup of the control and it will...

How do you tell when a tap is getting dull (before it breaks)?

i found i need to keep track of how many times i've used the tap and
sometimes turn it in my fingers to feed the edge. i tap on a manual mill
and never had a cnc to do the tapping.

Do you do any special hole prep for rigid tapping?

i never had any trouble drilling to tap size on the chart, been able to tap
up til 3/4" tap. after that the miil wasn't strong enough. and i've always
use tapping oil.( usually tap magic or such)

Is there anything that a newbie should know before plunging his first tap into some steel?

just correct holes size and tappng oil. if your doing thru holes, i like to
use spiral taps. it throws the shavings down so they don't get in the way of the tap.
if no spiral tap, i used a tapered tap. and as you said it also matters what you're tapping. 4140, stainless or aluminum.
hope this helps in some way.

Thanks
John

BigJohnT wrote:

I finally have a VMC that is capable of rigid tapping. At this time it is not running EMC but at the first hiccup of the control and it will...

How do you tell when a tap is getting dull (before it breaks)?

If you have a spindle load meter, that might give some indication. Otherwise, the taps will likely break due to accumulation or binding of chips before they wear out. Tapping at higher speeds produces much less wear on the taps, at least in softer materials like aluminum they seem to last forever.

Do you do any special hole prep for rigid tapping?

For thin materials, I use combination drill-taps, so you just plunge one tool in and do the whole job - spot, drill and tap. For thicker materials I drill as usual and then use a spiral point tap to push the chips ahead. For blind holes I use spiral flute taps that bring the chips out like a twist drill. On these, you need to clear the tap's flutes with a brush after each hole. A special tapping fluid seems to make a big difference, I use Alum-Tap.

Is there anything that a newbie should know before plunging his first tap into some steel?

Yes, probably try it in aluminum, first. Don't be afraid to use MUCH higher spindle speeds than you ever thought tapping could be done at. I was doing some 10-32 tapping at 600+ RPM and 4-40 at 1200 RPM
on my machine.

And, of course, if using EMC2, use Halscope first to check the Z-axis following error during the spindle reversal. If the error is too much, you can reduce it by using a lower spindle speed or adding filtering to soften the rate at which the spindle reverses.

Jon

Just wanted to (again) thank the LinuxCNC gurus who got rigid tapping working!
I just did 480 4-40 holes using a combo drill-tap and it took about 2 hours, much of
it just swapping the pieces.

I used to dread doing stuff with a lot of threaded holes. The best was to
use the CNC to position the work under the spindle and then manually
tap the holes. This at least put the tap vertical and centered over the
hole, but was still a LOT of work.

With rigid tapping and the combo drill-taps it is fast, and I can do thousands of
holes on one tap unless I make a stupid setup mistake. I do the 4-40's
at 1000 RPM.

Jon

Greetings:

I am planning on adding rigid taping to my mill. I am running LinuxCNC 2.4.6 on an 800MHz single core processor. The mill is hooked up via a standard parallel port. I have the latency for the mill set at 15uS and am able to get 75ipm rapids without any problems. The top speed of my mill spindle is 5000 rpm.

I am contemplating purchasing an E3 encoder from US Digital. The question I have is what CPR should I order? The encoder can be ordered in CPR levels of 64, 100, 200, 400, 500, 512, 1000, 1024, 1800, 2000, 2048 and 2500. I am contemplating being able to rigid tap in the 4-40, 6-32, 10-32, and 1/4-20 thread ranges. What is the smallest CPR that would still provide enough resolution for rigid tapping? At what point does higher CPR become overkill? At 15uS latency, is a parallel port up to the task of doing rigid tapping? Should I give up on the parallel port and invest in an FPGA based solution?

I am trying to understand what all of the various trade-offs are. I am not against purchasing additional hardware (if needed), but I really do not know if additional hardware is actually needed. If not needed, I would just as soon save the money.

Any insight would be appreciated.

-Wayne

at 5000 RPM and a 64 line (256 count/turn) encoder, the maximum count rate is ~21 KHz or about 47 usec per count.

with a 33 KHz base thread (twice latency = 30 usec) and a good encoder this should be just
readable via the parallel port at 5000 RPM

Also its very unlikely you will get anywhere near 5000 RPM while tapping

I dont think there is much advantage to higher resolution on spindle encoders than 256 counts/turn

waynegramlich wrote:

Greetings:

I am planning on adding rigid taping to my mill.
-Wayne

Oh, one other area that you need to be concerned about. The Z axis needs to
be able to follow the spindle speed changes. So, either the spindle reversals
need to be moderated or the Z axis needs to have very quick acceleration.
I had to put a filter into the spindle speed commands to slow down the reversal
so the Z axis could keep up.

If you have a stepper axis setup, then it is a bit hard to know if there are
any velocity lags in your stepper drivers. So, it is just a little hard to know
exactly how well the axes are following the commands to sync to the
spindle.

Jon

waynegramlich wrote:

Greetings:

What is the smallest CPR that would still provide enough resolution for rigid tapping? At what point does higher CPR become overkill? At 15uS latency, is a parallel port up to the task of doing rigid tapping? Should I give up on the parallel port and invest in an FPGA based solution?


-Wayne

I have been doing rigid tapping in 2-56 through 10-32 sizes in aluminum on my Bridgeport.
There's no way to attach an encoder to the spindle, so I use the teeth of the bull gear as an
encoder disc. It has 81 teeth, so that is equivalent to an 81 cycle/rev encoder disk, giving
324 quadrature counts. This has worked fine. I suspect the 64 cycle/rev encoder will
also work fine.

Peter Wallace has given the calculation for the spindle speeds with a 64 CPR encoder.
You may want to also set up a spindle speed display on screen for the spindle RPM,
so you would want the encoder counter to be able to keep up at the highest spindle
speed you can do. So, that sets the upper limit on the encoder resolution.

Jon