- Marcus,

Thanks. I intend to tap a lot of holes, so anything to speed it up

would be helpful. also I am tapping platic, so I don't expect many

broken taps. However, I think your pointing out that CNC'g to each

hole position helps, and the mill keeps the tap vertical. I indeed

appreciate you sharing your extensive experience in approaching this

particular problem. Your approach using the drill chuck in an end mill

seems like a notch or two better than what I did the last time, which

was mount a 4-jaw chuck on the spindle, and use it to guide a tap

handle as I turned the handle and tap manually.

Neil--- In SherlineCNC@yahoogroups.com, "Marcus and Eva" <implmex@a...> wrote:

> Hi Tony and others:

> I've got a CNC that has the whole nine yards on it (rigid

tapping, which

> means the spindle can be timed to rotate at the correct speed while

the Z

> axis drives down at the right rate) and you know how I end up doing

most of

> my tapping???

> I stick a drill chuck on a stubby arbor into an end mill holder.

> I position the drill chuck with tap in it over the hole.

> I drop the spindle down till the tap is within 1/4" of the top of

the hole.

> I release the setscrew that holds the stub arbor in the endmill

holder so

> the tap and drill chuck can drop down.

> I spin the chuck by hand to get the tap started.

> I back it out by hand and move to the next hole.

> I finish the holes with a tap wrench by hand.

>

> Why do I do this, you ask, when I've got the full meal deal on the super

> dooper CNC???

> Because it's faster for small numbers of holes, and because it's a

lot less

> risky.

> Setting up for production tapping can be a royal pain in the rear.

> It just ain't worth it for only a few holes, especially if you bust

a tap!!!

>

> It's awfully tempting to think you'll reap tremendous benefits by

harnessing

> all this cool technology...I did it too when I first got the machine.

> Interestingly, I find myself moving away from CNC for many

operations as I

> get better at identifying which ones will be time wasters.

> I'd find myself piddling away hours of time to do a 5 minute job, and

> holemaking has been one of the worst offenders for my kind of work

> (moldmaking).

> I had to EDM out a lot more broken taps too, ususally from slamming

the tap

> into a chip at the bottom of the hole.

>

> I'd recommend staying away from tapping heads and fancy CNC rigs for the

> homebrew setup unless you've got hundreds or thousands of holes to

tap on a

> typical job.

> Anything less than 30 holes or so, and I don't bother with the tapping

> setup...even when I've co-ordinate drilled the holes in the CNC.

> Of course, I still position the tap over all the locations with the CNC.

>

> Cheers

>

> Marcus - johnclif@... wrote:
>

***********************

> Okay... how do you mill from the bottom up with this threadmill,

> since you can't put the threadmill into the hole before you start

> cutting. You could turn the piece upside down and mill from the

> bottom DOWN, but what does that get you on a thru-hole? If the hole

> is blind, I don't see how you can use this threadmill in any

> direction but down.

>

> I also see that it would require the Z feed speed to be very-well

> syncronized with RPM. In short, seems like it would work better with

> professional machines than with a CNC'd Sherline.

>

> - jgc

Hello John,

A typical threadmill has 2 or 4 cutting points sticking out sideways

beyond the shank. The diameter between points is smaller than the

predrilled hole to be tapped. The #4 threadmill that I use measures

about 0.080 inches from point to point.

For a 4-40 thread, I drill a 0.089 inch diameter hole, just as I would

for common tapping. Then I look up the outside diameter of a 4-40 thread

(something like 0.112 inch). I lower the threadmill, centered on the

hole, to just above the bottom. Then move it to the left 0.016 inches so

the teeth are cutting into the wall. Then do the counter clockwise helix

while ascending out of the hole.

Below is a section of Gcode, written for TurboCnc 3.1a, that thread

mills four 4-40 holes. This is done with a subroutine using relative

motion.

EMC does not do subroutines so you would have to embed the helix routine

in four places rather than call it as a subroutine.

Tom Hubin

thubin@...

**************************************

M00 ; File: Cube05D\Cage\Drill.cnc 5 October 2004

G90 ; absolute

G70 ; inches

M00 ; use 1.9370" x 1.9370" x 1.7323" cage

M00 ; ref corner is (right, back, bottom) = (+0.9685, +0.0, -1.7323)

M00 ; (0,0,0) is (center, rear, top)

M00 ; Load small center drill and touch surface

G92 Z 0.0 ; define surface as z=0

G00 Z 0.040 ; raise the bit

M00 ; Tighten bit and start spindle 2800 RPM

; four tap 4-40 holes

G00 X -0.6500 Y -0.1185

G82 X -0.7500 Y -0.2185 Z -0.030 R 0.040 F 1.0 #250

G00 X +0.8500 Y -0.1185

G82 X +0.7500 Y -0.2185 Z -0.030 R 0.040 F 1.0 #250

G00 X -0.6500 Y -1.6185

G82 X -0.7500 Y -1.7185 Z -0.030 R 0.040 F 1.0 #250

G00 X +0.8500 Y -1.6185

G82 X +0.7500 Y -1.7185 Z -0.030 R 0.040 F 1.0 #250

M00 ; Load #43 (0.089 inch) drill and touch surface

G92 Z 0.0 ; define surface as z=0

G00 Z 0.040 ; raise the bit

M00 ; Tighten bit and start spindle 2800 RPM

; four tap 4-40 holes

G00 X -0.6500 Y -0.1185

G83 X -0.7500 Y -0.2185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

G00 X +0.8500 Y -0.1185

G83 X +0.7500 Y -0.2185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

G00 X -0.6500 Y -1.6185

G83 X -0.7500 Y -1.7185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

G00 X +0.8500 Y -1.6185

G83 X +0.7500 Y -1.7185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

M00 ; Load #4 threadmill and touch surface

G92 Z 0.0 ; define surface as z=0

G00 Z 0.040 ; raise the bit

M00 ; Tighten bit and start spindle 2800 RPM

; four tap 4-40 holes

G00 X -0.650 Y -0.1185

G00 X -0.750 Y -0.2185

N210 M60 #2000 ; threadmill helix

G00 X +0.850 Y -0.1185

G00 X +0.750 Y -0.2185

N220 M60 #2000 ; threadmill helix

G00 X -0.650 Y -1.6185

G00 X -0.750 Y -1.7185

N230 M60 #2000 ; threadmill helix

G00 X +0.850 Y -1.6185

G00 X +0.750 Y -1.7185

N240 M60 #2000 ; threadmill helix

M02 ; finished

;**************************************************

N2000 ; 0.080 inch threadmill helix for 4-40 holes

G01 Z -0.275 F 1.0 ; start just above bottom of hole

G91 ; start incremental mode

G01 X -0.0160 F 1.0 ; move to left side of hole

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.250

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.225

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.200

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.175

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.150

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.125

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.100

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.075

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.050

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.025

G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.000

G01 X +0.0160 ; move to center of hole

G90 ; restore absolute mode

G00 Z +0.200 ; exit the hole

M62 ; end of threadmill helix subroutine