I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html

On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote:

I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html


By chance I just finished drill and tap to 3/8 on four holes in AL
1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips
that fed out well and broke every two inch or so. Used my coolant
mister at a heavy flow.

Karl

On Sun, 26 Sep 2010 17:34:44 -0500, Karl Townsend
wrote:

On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote:

I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html


By chance I just finished drill and tap to 3/8 on four holes in AL
1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips
that fed out well and broke every two inch or so. Used my coolant
mister at a heavy flow.

Karl

sorry you had two more queries.

I used a solid holder, your floating holder would be nice.

Spot drill if you need to hold +/- .002 location, stub drill maybe +/-
..005, regular drill maybe +/- .010 or worse. So how accurate
determines answer.

Karl

On 2010-09-27, Gene wrote:
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote:

I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

That depends on the drill and the material. HSS drill? Maybe 2500 RPM
and maybe .005 per rev feed. That is a bit conservative, but I'd
prefer to finish without a lot of tool changing. Pecking once will
probably be sufficient.

Not bad. 80 rev per secons and 0.005 per rev means 0.4 inch per
second.

Would the stringy chips want to wrap around the drill bit?

Be wary, though, of scoring "good deals" in material. If this isn't
cast tooling plate, but some soft sticky stuff more akin to 1100,
you'll have your hands full. Use a cutting fluid.

I will use flood coolant in large amounts.

his plate alteady has a few smaller holes drilled and tapped.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

Absolutely, if nothing else, done properly, they provide the chamfer
for the finished thread.

Great. I am thinking, use a spotting drill, and drill a full diameter
hole that is perhaps 1/8" deep. That would provide good centering.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html

Sure. Go for it. However, again, if you have inherited some suspicious
material, say one of the 6xxx materials.... you'll dull taps VERY
quickly and a tap burner or scrap will be in your immediate future.

Well, it is already tapped, so it is tappable.

ix

On 2010-09-26, Karl Townsend wrote:
On Sun, 26 Sep 2010 17:34:44 -0500, Karl Townsend
wrote:

On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote:

I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html


By chance I just finished drill and tap to 3/8 on four holes in AL
1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips
that fed out well and broke every two inch or so. Used my coolant
mister at a heavy flow.

Karl

sorry you had two more queries.

I used a solid holder, your floating holder would be nice.

Spot drill if you need to hold +/- .002 location, stub drill maybe +/-
.005, regular drill maybe +/- .010 or worse. So how accurate
determines answer.

Karl


I will use a spot drill indeed. Full diameter holes with spot drill,
perhaps 1/8" deep, to provide guidance for the regular drill.

i

On 2010-09-26, Karl Townsend wrote:
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote:

I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html


By chance I just finished drill and tap to 3/8 on four holes in AL
1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips
that fed out well and broke every two inch or so. Used my coolant
mister at a heavy flow.

Karl

Pretty cool. You feed 5.1 is how many inches per second?

Someone suggested 0.4 IPS, which makes some sense to me.

i

On Sun, 26 Sep 2010 21:24:40 -0500, Ignoramus24898
wrote:

On 2010-09-26, Karl Townsend wrote:
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote:

I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html


By chance I just finished drill and tap to 3/8 on four holes in AL
1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips
that fed out well and broke every two inch or so. Used my coolant
mister at a heavy flow.

Karl

Pretty cool. You feed 5.1 is how many inches per second?

Someone suggested 0.4 IPS, which makes some sense to me.

i

That's 5.1 IPM. I just looked at the math, probably could have doubled
the feed. Only four holes, chips were feeding, don't **** with it.

Karl

On 2010-09-27, Karl Townsend wrote:
On Sun, 26 Sep 2010 21:24:40 -0500, Ignoramus24898
wrote:

On 2010-09-26, Karl Townsend wrote:
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898
wrote:

I bought a couple of 3/4" thick aluminum fixture plates.

http://igor.chudov.com/tmp/Fixture-Plate.jpg

It was a local sale.

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html


By chance I just finished drill and tap to 3/8 on four holes in AL
1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips
that fed out well and broke every two inch or so. Used my coolant
mister at a heavy flow.

Karl

Pretty cool. You feed 5.1 is how many inches per second?

Someone suggested 0.4 IPS, which makes some sense to me.

i

That's 5.1 IPM. I just looked at the math, probably could have doubled
the feed. Only four holes, chips were feeding, don't **** with it.

Just trying to do the math. 5 IPM, means one 1" hole drilled in 12
seconds, so it amounts to about 20 seconds per hole with rapids and
everything. 200 holes, means 4,000 seconds, a little over an
hour. Probably can run unsupervised. Not too bad.

How bad were the chips?

i

Great. I am thinking, use a spotting drill, and drill a full diameter
hole that is perhaps 1/8" deep. That would provide good centering.




If you use 60 degree center drill and go to a depth of half the hole
diameter of the 3/8 thread diameter the finished hole will have a nice
chamfer on it with no need for any deburring.

John

Ignoramus24898 writes:

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

How frequently do you break taps? If you're not an utterly reliable
tapper, you'll never be able to complete this job. Consider that if your
workpiece is ruined by breaking a tap, then you must succeed at all 200 in
a row. For a 90 percent chance of success, then, each individual hole must
be tapped with a 99.95 percent chance of success.

If you break a tap, say, once every hundred holes, then you have an 87
percent chance of failure on this piece (1.0 - 0.99**200 = 0.87).

Now you know why these cost $$$$:

http://www.edmundoptics.com/onlineca...productID=2929

On Sun, 26 Sep 2010 21:23:33 -0500, Ignoramus24898 wrote:
On 2010-09-26, Karl Townsend wrote:

Spot drill if you need to hold +/- .002 location, stub drill maybe +/-
.005, regular drill maybe +/- .010 or worse. So how accurate determines
answer.

I will use a spot drill indeed. Full diameter holes with spot drill,
perhaps 1/8" deep, to provide guidance for the regular drill.

Is a "spot drill" the same thing as a "center drill"? (it kind of sounds
like it, from Karl's info here.)

Thanks,
Rich

On Sun, 26 Sep 2010 21:24:40 -0500, Ignoramus24898 wrote:
On 2010-09-26, Karl Townsend wrote:
On Sun, 26 Sep 2010 16:41:07 -0500, Ignoramus24898

Some questions.

1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.

2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.

3. For tapping, can I safely use a ER colleted floating tap holder that
has a little bit of vertical internal travel. Like this one:

http://www.maritool.com/p67/ER25-Flo...duct_info.html

By chance I just finished drill and tap to 3/8 on four holes in AL 1.25"
deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed
out well and broke every two inch or so. Used my coolant mister at a
heavy flow.

Pretty cool. You feed 5.1 is how many inches per second?

Someone suggested 0.4 IPS, which makes some sense to me.

This makes me wonder: Is there a machine where a machinist could make
one part "by hand", i.e., in the normal way you'd use a regular mill
or whatever, but where the machine could record the machinist's actions,
and then "play them back" for the next part? Or is it only possible to
drive an NC by writing a string of textual commands?

Thanks,
Rich

On Sep 26, 10:23*pm, Ignoramus24898

Spot drill if you need to hold +/- .002 location, stub drill maybe +/-
.005, *regular drill maybe +/- .010 or worse. So how accurate
determines answer.

Karl

I will use a spot drill indeed. Full diameter holes with spot drill,
perhaps 1/8" deep, to provide guidance for the regular drill.

i

If I were doing this on a manual mill, I would spot drill with a drill
whose diameter is about the size of the web of the drill used for the
hole.

Dan

On Sun, 26 Sep 2010 23:32:26 -0700, Rich Grise
wrote:

On Sun, 26 Sep 2010 21:23:33 -0500, Ignoramus24898 wrote:
On 2010-09-26, Karl Townsend wrote:

Spot drill if you need to hold +/- .002 location, stub drill maybe +/-
.005, regular drill maybe +/- .010 or worse. So how accurate determines
answer.

I will use a spot drill indeed. Full diameter holes with spot drill,
perhaps 1/8" deep, to provide guidance for the regular drill.

Is a "spot drill" the same thing as a "center drill"? (it kind of sounds
like it, from Karl's info here.)

Thanks,
Ric

No, they are different. A spot drill looks like a drill bit with a
special grind point.

How bad were the chips?

I had no trouble with my mystery metal AL. Some AL is a stone bitch to
feed the chips up the drill bit, others work great. As nearly all my
metal falls in the mystery metal class, i can't tell you which grade
is best.

You should feed maybe twice as fast as my small run.

Karl

This makes me wonder: Is there a machine where a machinist could make
one part "by hand", i.e., in the normal way you'd use a regular mill
or whatever, but where the machine could record the machinist's actions,
and then "play them back" for the next part? Or is it only possible to
drive an NC by writing a string of textual commands?

My control has a "teach" mode to record points but you still eidt to
make a program. I never used one but the bridegeport protrack was
supposed to do this.

Karl

On 2010-09-27, Karl Townsend wrote:

How bad were the chips?

I had no trouble with my mystery metal AL. Some AL is a stone bitch to
feed the chips up the drill bit, others work great. As nearly all my
metal falls in the mystery metal class, i can't tell you which grade
is best.

You should feed maybe twice as fast as my small run.

Karl


Karl, thanks. I will try on some aluminum junk that I have, first.

Tapping, as Richard noted, may be a challenge.

What tap would you recommend for this (tapping aluminum)?

Thanks

i

On 2010-09-27, Richard J Kinch wrote:
Ignoramus24898 writes:

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

How frequently do you break taps? If you're not an utterly reliable
tapper, you'll never be able to complete this job. Consider that if your
workpiece is ruined by breaking a tap, then you must succeed at all 200 in
a row. For a 90 percent chance of success, then, each individual hole must
be tapped with a 99.95 percent chance of success.

If you break a tap, say, once every hundred holes, then you have an 87
percent chance of failure on this piece (1.0 - 0.99**200 = 0.87).

Now you know why these cost $$$$:

http://www.edmundoptics.com/onlineca...productID=2929


Richard, I was hoping that I would tap on my CNC mill, so whatever
process I do, would be repeatable and not as random as manual tapping.

i

On Sep 27, 8:26*am, Ignoramus21149 ignoramus21...@NOSPAM.
21149.invalid wrote:
On 2010-09-27, Richard J Kinch wrote:





Ignoramus24898 writes:

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

How frequently do you break taps? *If you're not an utterly reliable
tapper, you'll never be able to complete this job. Consider that if your
workpiece is ruined by breaking a tap, then you must succeed at all 200 in
a row. *For a 90 percent chance of success, then, each individual hole must
be tapped with a 99.95 percent chance of success.

If you break a tap, say, once every hundred holes, then you have an 87
percent chance of failure on this piece (1.0 - 0.99**200 = 0.87).

Now you know why these cost $$$$:

http://www.edmundoptics.com/onlineca...t.cfm?productI...

Richard, I was hoping that I would tap on my CNC mill, so whatever
process I do, would be repeatable and not as random as manual tapping.

i- Hide quoted text -

- Show quoted text -

For aluminum, you may want to use a Thread Forming Tap, instead of a
Thread Cutting Tap...Since you will be using coolant/cutting fluid,
the going will be much easier, and the thread will be stronger. A
thread forming tap has the additional advantage of no chips.

_kevin

"Ignoramus21149" wrote in message
...
On 2010-09-27, Karl Townsend wrote:

How bad were the chips?

I had no trouble with my mystery metal AL. Some AL is a stone bitch to
feed the chips up the drill bit, others work great. As nearly all my
metal falls in the mystery metal class, i can't tell you which grade
is best.

You should feed maybe twice as fast as my small run.

Karl


Karl, thanks. I will try on some aluminum junk that I have, first.

Tapping, as Richard noted, may be a challenge.

What tap would you recommend for this (tapping aluminum)?

Thanks

i

If they are through holes, I would go with a gun tap - they push the chips
ahead of the tap. I have a Procunier tapping head you could borrow for a
week or so if that would help. I've tapped a bunch of 0-80 and 4-40 holes
with nary a broken tap so 5/16" shouldn't be a problem for that style of
head.

Mike

On 2010-09-27, karchiba wrote:
For aluminum, you may want to use a Thread Forming Tap, instead of a
Thread Cutting Tap...Since you will be using coolant/cutting fluid,
the going will be much easier, and the thread will be stronger. A
thread forming tap has the additional advantage of no chips.

That's a good idea. Would you say, with a proper tin coated tap like
this, and using a letter S drill, the 3/8" holes can be tapped
consistently on my CNC mill?

i

On 2010-09-27, Mike Henry wrote:

"Ignoramus21149" wrote in message
...
On 2010-09-27, Karl Townsend wrote:

How bad were the chips?

I had no trouble with my mystery metal AL. Some AL is a stone bitch to
feed the chips up the drill bit, others work great. As nearly all my
metal falls in the mystery metal class, i can't tell you which grade
is best.

You should feed maybe twice as fast as my small run.

Karl


Karl, thanks. I will try on some aluminum junk that I have, first.

Tapping, as Richard noted, may be a challenge.

What tap would you recommend for this (tapping aluminum)?

Thanks

i

If they are through holes, I would go with a gun tap - they push the chips
ahead of the tap. I have a Procunier tapping head you could borrow for a
week or so if that would help. I've tapped a bunch of 0-80 and 4-40 holes
with nary a broken tap so 5/16" shouldn't be a problem for that style of
head.


Mike, did you use that head on a CNC mill?

Karl, thanks. I will try on some aluminum junk that I have, first.

Tapping, as Richard noted, may be a challenge.

What tap would you recommend for this (tapping aluminum)?

I don't agree with Richard's analysis. His method assumes the
probabilty of a broken tap is the same on every hole. In fact, once
you've set up proper conditions and selected a top quality tap the
probablity of breaking goes with wear. Taps used in machines last FAR
longer than hand taps.

I use OSG brand taps. Gun flute on thru hole, spiral flute on blind
hole. I forget, you aren't set up for rigid tapping??

Both your tension/compression tap holder and the procunier can be set
up in your CNC. But, its tricky. You've got to match feeds and speeds
to where the tap wants to be.

Karl

On 2010-09-27, Karl Townsend wrote:

Karl, thanks. I will try on some aluminum junk that I have, first.

Tapping, as Richard noted, may be a challenge.

What tap would you recommend for this (tapping aluminum)?

I don't agree with Richard's analysis. His method assumes the
probabilty of a broken tap is the same on every hole. In fact, once
you've set up proper conditions and selected a top quality tap the
probablity of breaking goes with wear. Taps used in machines last
FAR longer than hand taps.

OK, good to hear.

I use OSG brand taps. Gun flute on thru hole, spiral flute on blind
hole. I forget, you aren't set up for rigid tapping??

Both your tension/compression tap holder and the procunier can be set
up in your CNC. But, its tricky. You've got to match feeds and speeds
to where the tap wants to be.

I understand, yes. If I run the spindle at, say, 200-300 RPM, then it
would take me about 0.2 seconds to stop the spindle, so about one
revolution. The floating tap holder should be able to take care of
that. You think ER16 collets would hold a tap well enough?

i

On 2010-09-27, Ignoramus21149 wrote:
On 2010-09-27, Karl Townsend wrote:

Karl, thanks. I will try on some aluminum junk that I have, first.

Tapping, as Richard noted, may be a challenge.

What tap would you recommend for this (tapping aluminum)?

I don't agree with Richard's analysis. His method assumes the
probabilty of a broken tap is the same on every hole. In fact, once
you've set up proper conditions and selected a top quality tap the
probablity of breaking goes with wear. Taps used in machines last
FAR longer than hand taps.

OK, good to hear.

I use OSG brand taps. Gun flute on thru hole, spiral flute on blind
hole. I forget, you aren't set up for rigid tapping??

Both your tension/compression tap holder and the procunier can be set
up in your CNC. But, its tricky. You've got to match feeds and speeds
to where the tap wants to be.

I understand, yes. If I run the spindle at, say, 200-300 RPM, then it
would take me about 0.2 seconds to stop the spindle, so about one
revolution. The floating tap holder should be able to take care of
that. You think ER16 collets would hold a tap well enough?

I wrote a G-code subroutine to do it. To run safely, it MUST have a
floating tap holder that can take up the slack of the tap that moves
off position, while the spindle is reversed.

(Tap a hole with a floating holder)
Otap_with_floating_holder sub
#depth = #1 (Hole Depth)
#tpi = #2 (Threads per Inch)
#rpm = #3 (RPM of the spindle, EXACTLY MEASURED)
#safez = #4 (Safe Height)

#frate = [#rpm / #tpi]

M3 (Forward)
G1 Z#depth F#frate
M4 (Reverse)
G1 Z#safez F#frate
M3 (Forward again)

Otap_with_floating_holder endsub
M2

On Sep 26, 11:11*pm, Richard J Kinch wrote:
Ignoramus24898 writes:

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

How frequently do you break taps? *If you're not an utterly reliable
tapper, you'll never be able to complete this job.

So, make threaded inserts of steel, for oversized holes (stepped would
be good) with a bit of loctite. The accuracy of a screw position
isn't
critical, I trust.

Of course, to churn out inserts might require a CNC lathe... or a
turret lathe.

On Mon, 27 Sep 2010 07:12:36 -0500, Karl Townsend wrote:
On Sun, 26 Sep 2010 23:32:26 -0700, Rich Grise
On Sun, 26 Sep 2010 21:23:33 -0500, Ignoramus24898 wrote:
On 2010-09-26, Karl Townsend wrote:

Spot drill if you need to hold +/- .002 location, stub drill maybe +/-
.005, regular drill maybe +/- .010 or worse. So how accurate
determines answer.

I will use a spot drill indeed. Full diameter holes with spot drill,
perhaps 1/8" deep, to provide guidance for the regular drill.

Is a "spot drill" the same thing as a "center drill"? (it kind of sounds
like it, from Karl's info here.)

No, they are different. A spot drill looks like a drill bit with a special
grind point.

Ah. Thanks. I sit in an office and fly a desk, while right outside my door
are a couple of machinists and weldors - on one side of the shop, we take
big pieces of metal and turn them into little pieces of metal, and on the
other side, we take small pieces of metal and turn them into big pieces
of metal. :-)

On break, the only people I have to talk to, other than the boss and his
secretary, are the machinists - When I'm chatting someone up, I like to
be able to speak the same language as they. :-)

I do know what "spot-facing" is, however. ;-)

Thanks!
Rich

On Mon, 27 Sep 2010 05:06:02 -0700, wrote:
On Sep 26, 10:23*pm, Ignoramus24898

Spot drill if you need to hold +/- .002 location, stub drill maybe +/-
.005, *regular drill maybe +/- .010 or worse. So how accurate
determines answer.

I will use a spot drill indeed. Full diameter holes with spot drill,
perhaps 1/8" deep, to provide guidance for the regular drill.

If I were doing this on a manual mill, I would spot drill with a drill
whose diameter is about the size of the web of the drill used for the
hole.

Do people use the terms "drill" and "drill bit" almost interchangeably?

To me, the "drill" is the part with the motor, that turns the "bit."

Am I wrong?

Thanks,
Rich

On Mon, 27 Sep 2010 07:19:21 -0500, Karl Townsend wrote:

How bad were the chips?

I had no trouble with my mystery metal AL. Some AL is a stone bitch to
feed the chips up the drill bit, others work great. As nearly all my metal
falls in the mystery metal class, i can't tell you which grade is best.

You should feed maybe twice as fast as my small run.

Once, after hours, I found some really spiffy pieces of aluminum out in
back next to the bandsaw. I wanted to make a trinket, and the resident
machinist taught me how to use a mill - I was astonished how much metal
he could hog off that aluminum block; Previously, as a hobbyist, I had
used about a quarter the feed rate this guy was getting away with.

I once got tasked to drill a couple of 1/2" holes in a 3/16" plate of
304SS. I din't even know you _could_ drill 304SS with an ordinary
twist drill, but again, my coach(es) said, "GO FOR IT!" I really bore
down on that handle thingie that extends the quill, and the stainless
just gave way. I heard that sound that you hear when one mongo chip
is being produced, and it felt almost like the drill was pulling itself
into the work - I was through 3/16 of metal in a matter of seconds,
almost effortlessly!

So, I guess I'd have to admit, when I'm playing with metal, I should be
more aggressive with my cuts. :-)

I once saw a guy deburr a steel part with an ordinary pocket knife. Does
that dull the knife?

How can steel cut steel? Howcome the part doesn't cut the bit?

Thanks,
Rich

On 09/27/2010 12:40 PM, Ignoramus21149 wrote:

I wrote a G-code subroutine to do it. To run safely, it MUST have a
floating tap holder that can take up the slack of the tap that moves
off position, while the spindle is reversed.

(Tap a hole with a floating holder)
Otap_with_floating_holder sub
#depth = #1 (Hole Depth)
#tpi = #2 (Threads per Inch)
#rpm = #3 (RPM of the spindle, EXACTLY MEASURED)
#safez = #4 (Safe Height)

#frate = [#rpm / #tpi]

M3 (Forward)
G1 Z#depth F#frate
M4 (Reverse)
G1 Z#safez F#frate
M3 (Forward again)

Otap_with_floating_holder endsub
M2

Well, this all SOUNDS good, but in fact, there is NO connection, at all,
between the spindle and the Z feed. You'd have to do the first test
holes carefully to make sure you get the desired depth of tapping.
The spindle is running at whatever speed it is, and the Z infeed goes at
the programmed rate. But, at the end, it is only the Z depth that
determines when to reverse. NOT, the number of turns the tap has fed
into the work.

Still, this is likely to work, assuming the springs on the tap holder
are strong enough to start the tap into the work promptly.

And, you won't believe what a MESS this will make, if you ever mess up
and have the spindle running at the wrong speed for the calculated
feedrate. been there, done that!

Jon

On Mon, 27 Sep 2010 07:22:47 -0500, Karl Townsend wrote:

This makes me wonder: Is there a machine where a machinist could make one
part "by hand", i.e., in the normal way you'd use a regular mill or
whatever, but where the machine could record the machinist's actions, and
then "play them back" for the next part? Or is it only possible to drive
an NC by writing a string of textual commands?

My control has a "teach" mode to record points but you still eidt to make
a program. I never used one but the bridegeport protrack was supposed to
do this.


Thanks; I was just curious, but it sounds like a fascinating opportunity
for a geek like me (microprocessor programmer) who dabbles in mechanical
stuff...

Thanks!
Rich

On 09/27/2010 10:13 AM, Ignoramus21149 wrote:
On 2010-09-27, wrote:
For aluminum, you may want to use a Thread Forming Tap, instead of a
Thread Cutting Tap...Since you will be using coolant/cutting fluid,
the going will be much easier, and the thread will be stronger. A
thread forming tap has the additional advantage of no chips.

That's a good idea. Would you say, with a proper tin coated tap like
this, and using a letter S drill, the 3/8" holes can be tapped
consistently on my CNC mill?

i

You use an entirely different drill size (much larger) for a thread
forming tap. The workpiece is pushed out of the peaks to form the
valleys. The tap manufacturer should be able to recommend the correct
drill size.

Jon

On 2010-09-27, Jon Elson wrote:
On 09/27/2010 12:40 PM, Ignoramus21149 wrote:

I wrote a G-code subroutine to do it. To run safely, it MUST have a
floating tap holder that can take up the slack of the tap that moves
off position, while the spindle is reversed.

(Tap a hole with a floating holder)
Otap_with_floating_holder sub
#depth = #1 (Hole Depth)
#tpi = #2 (Threads per Inch)
#rpm = #3 (RPM of the spindle, EXACTLY MEASURED)
#safez = #4 (Safe Height)

#frate = [#rpm / #tpi]

M3 (Forward)
G1 Z#depth F#frate
M4 (Reverse)
G1 Z#safez F#frate
M3 (Forward again)

Otap_with_floating_holder endsub
M2

Well, this all SOUNDS good, but in fact, there is NO connection, at
all, between the spindle and the Z feed.

The only connection is that I measure the speed of the spindle with a
handheld tachometer, and then calculate the feed.

You'd have to do the first test holes carefully to make sure you get
the desired depth of tapping. The spindle is running at whatever
speed it is, and the Z infeed goes at the programmed rate. But, at
the end, it is only the Z depth that determines when to reverse.
NOT, the number of turns the tap has fed into the work.

Absolutely.

Still, this is likely to work, assuming the springs on the tap holder
are strong enough to start the tap into the work promptly.

And, you won't believe what a MESS this will make, if you ever mess up
and have the spindle running at the wrong speed for the calculated
feedrate. been there, done that!

What will happen, it will tear the tap out of the collet?

Anyway, obviously rigid tapping, optionally with the floating holder,
is the way to go.

i

On 2010-09-27, Jon Elson wrote:
On 09/27/2010 10:13 AM, Ignoramus21149 wrote:
On 2010-09-27, wrote:
For aluminum, you may want to use a Thread Forming Tap, instead of a
Thread Cutting Tap...Since you will be using coolant/cutting fluid,
the going will be much easier, and the thread will be stronger. A
thread forming tap has the additional advantage of no chips.

That's a good idea. Would you say, with a proper tin coated tap like
this, and using a letter S drill, the 3/8" holes can be tapped
consistently on my CNC mill?

i

You use an entirely different drill size (much larger) for a thread
forming tap. The workpiece is pushed out of the peaks to form the
valleys. The tap manufacturer should be able to recommend the correct
drill size.

Yep.

I will buy a form tap today at mcmaster, they say use letter S drill.

i

Rich Grise wrote:
On Mon, 27 Sep 2010 07:19:21 -0500, Karl Townsend wrote:

How bad were the chips?

I had no trouble with my mystery metal AL. Some AL is a stone bitch to
feed the chips up the drill bit, others work great. As nearly all my metal
falls in the mystery metal class, i can't tell you which grade is best.

You should feed maybe twice as fast as my small run.

Once, after hours, I found some really spiffy pieces of aluminum out in
back next to the bandsaw. I wanted to make a trinket, and the resident
machinist taught me how to use a mill - I was astonished how much metal
he could hog off that aluminum block; Previously, as a hobbyist, I had
used about a quarter the feed rate this guy was getting away with.

I once got tasked to drill a couple of 1/2" holes in a 3/16" plate of
304SS. I din't even know you _could_ drill 304SS with an ordinary
twist drill, but again, my coach(es) said, "GO FOR IT!" I really bore
down on that handle thingie that extends the quill, and the stainless
just gave way. I heard that sound that you hear when one mongo chip
is being produced, and it felt almost like the drill was pulling itself
into the work - I was through 3/16 of metal in a matter of seconds,
almost effortlessly!

So, I guess I'd have to admit, when I'm playing with metal, I should be
more aggressive with my cuts. :-)

And never ease off the pressure until you are
at depth or through the other side. Many steels
will work-harden in an instant if you let the
drill spin and not cut.

On 9/27/2010 3:08 PM, Rich Grise wrote:
On Mon, 27 Sep 2010 07:19:21 -0500, Karl Townsend wrote:

How bad were the chips?

I had no trouble with my mystery metal AL. Some AL is a stone bitch to
feed the chips up the drill bit, others work great. As nearly all my metal
falls in the mystery metal class, i can't tell you which grade is best.

You should feed maybe twice as fast as my small run.

Once, after hours, I found some really spiffy pieces of aluminum out in
back next to the bandsaw. I wanted to make a trinket, and the resident
machinist taught me how to use a mill - I was astonished how much metal
he could hog off that aluminum block; Previously, as a hobbyist, I had
used about a quarter the feed rate this guy was getting away with.

I once got tasked to drill a couple of 1/2" holes in a 3/16" plate of
304SS. I din't even know you _could_ drill 304SS with an ordinary
twist drill, but again, my coach(es) said, "GO FOR IT!" I really bore
down on that handle thingie that extends the quill, and the stainless
just gave way. I heard that sound that you hear when one mongo chip
is being produced, and it felt almost like the drill was pulling itself
into the work - I was through 3/16 of metal in a matter of seconds,
almost effortlessly!

So, I guess I'd have to admit, when I'm playing with metal, I should be
more aggressive with my cuts. :-)

I once saw a guy deburr a steel part with an ordinary pocket knife. Does
that dull the knife?

How can steel cut steel? Howcome the part doesn't cut the bit?

There's hard steel, and there's soft steel.
The hard steel cuts the soft steel.

--
I can see November from my front porch

On 2010-09-27, Richard J Kinch wrote:
Ignoramus24898 writes:

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

How frequently do you break taps? If you're not an utterly reliable
tapper, you'll never be able to complete this job. Consider that if your
workpiece is ruined by breaking a tap, then you must succeed at all 200 in
a row. For a 90 percent chance of success, then, each individual hole must
be tapped with a 99.95 percent chance of success.

If you break a tap, say, once every hundred holes, then you have an 87
percent chance of failure on this piece (1.0 - 0.99**200 = 0.87).

I think, with the proper coolant/lubricant, good gun (spiral
point) taps, and the consistency of the CNC, he might be able to do this
with no problems -- with a high quality tap and a good hard aluminum
alloy. I would either use a TapMagic for aluminum, or just use WD-40 in
aluminum.

Even better for the task would be a TapMatic tap head (which
would eliminate the problem of feeding in reverse as you back the tap
out). The thing with at least some models of TapMatic heads is a
friction clutch, which you set up with a brand new tap so is just barely
does not slip when cutting with the proper lubricant. Then, once the
tap starts getting dull, it will slip and you can change out the tap
*before* it breaks.

I've used this setup in a drill press with 1/4-20 HSS gun taps
with 1/4" steel (making an apron for an old DiAcro sheet metal shear).

Now you know why these cost $$$$:

http://www.edmundoptics.com/onlineca...productID=2929

Hmm ... the code which that website has which wants to know
where I live is a pain. I can't find the right things to turn on to get
it to accept my data (cookies and JavaScript on, and it still refuses to
admit that I've given it a value and keeps asking. It probably wants
flash, which I refuse to turn on.

So -- I had to start over and click the [dismiss] button to get
anywhere since it would not let me back out to the original starting
point.

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 2010-09-27, karchiba wrote:
On Sep 27, 8:26*am, Ignoramus21149 ignoramus21...@NOSPAM.
21149.invalid wrote:
On 2010-09-27, Richard J Kinch wrote:





Ignoramus24898 writes:

I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.

How frequently do you break taps? *If you're not an utterly reliable
tapper, you'll never be able to complete this job. Consider that if your
workpiece is ruined by breaking a tap, then you must succeed at all 200 in
a row. *For a 90 percent chance of success, then, each individual hole must
be tapped with a 99.95 percent chance of success.

If you break a tap, say, once every hundred holes, then you have an 87
percent chance of failure on this piece (1.0 - 0.99**200 = 0.87).

[ ... ]

Richard, I was hoping that I would tap on my CNC mill, so whatever
process I do, would be repeatable and not as random as manual tapping.

[ ... ]

For aluminum, you may want to use a Thread Forming Tap, instead of a
Thread Cutting Tap...Since you will be using coolant/cutting fluid,
the going will be much easier, and the thread will be stronger. A
thread forming tap has the additional advantage of no chips.

That is a good idea. However -- be sure to look up the right
drill size for a thread forming tap. It *has* to be larger than the
normal thread cutting tap's tap drill. You say 3/8" holes, but don't
say which thread pitch, so I can't look up the drill size. It can be
found in _Machinery's Handbook_.

The nearest to perfect size for a 1/4-20 tap happens to be a
metric size -- 5.7mm -- another argument for having drills of all kinds.

The proper size for 10-32 thread forming taps is a #17 -- from
your recently acquired number sized drill set.

Good Luck,
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 2010-09-27, Ignoramus21149 wrote:
On 2010-09-27, karchiba wrote:
For aluminum, you may want to use a Thread Forming Tap, instead of a
Thread Cutting Tap...Since you will be using coolant/cutting fluid,
the going will be much easier, and the thread will be stronger. A
thread forming tap has the additional advantage of no chips.

That's a good idea. Would you say, with a proper tin coated tap like
this, and using a letter S drill, the 3/8" holes can be tapped
consistently on my CNC mill?

I see that you've found the "Cold Form Tapping" chart in
_Machinery's Handbook_ -- and that you are going for 3/8-16 threads, and
65% full thread.

The final question is -- what is the proper lubricant for this
in aluminum? (And no -- *I* don't know the answer -- I hope someone
else here does.)

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 2010-09-27, Ignoramus21149 wrote:
On 2010-09-27, Karl Townsend wrote:

[ ... ]

I don't agree with Richard's analysis. His method assumes the
probabilty of a broken tap is the same on every hole. In fact, once
you've set up proper conditions and selected a top quality tap the
probablity of breaking goes with wear. Taps used in machines last
FAR longer than hand taps.

OK, good to hear.

I use OSG brand taps. Gun flute on thru hole, spiral flute on blind
hole. I forget, you aren't set up for rigid tapping??

Both your tension/compression tap holder and the procunier can be set
up in your CNC. But, its tricky. You've got to match feeds and speeds
to where the tap wants to be.

I understand, yes. If I run the spindle at, say, 200-300 RPM, then it
would take me about 0.2 seconds to stop the spindle, so about one
revolution. The floating tap holder should be able to take care of
that.

But you *really* should keep feeding according to the revolution
of the spindle on the index until it stops -- so your machine knows
where the tap is when it starts in reverse.

You think ER16 collets would hold a tap well enough?

The typical tapping head has a special chuck. It uses two ways
to hold the tap. A Jacobs Rubberflex type collet to assure
concentricity and a pair of plates with a combination left and right
hand threaded leadscrew connecting them to clamp down on the flats on
the end of the tap shank.

Some floating tap holders have similar chucks.

The main thing to consider is -- if it *does* slip and you are
doing rigid tapping, it will no longer be at the right depth for the
number of turns which the tap has taken.

I would look for something with the Jacobs tap chuck for this,
myself. And the Procunier or TapMatic tapping heads have them, along
with other features which make machine tapping easier -- including
automatic reversing when you start to back out of the hole -- while the
spindle is still turning clockwise. :-)

When doing tapping with a releasing tap holder in the bed turret
of my manual lathe, I've made tap holders which are simply the right
diameter for the shank of the tap, and a pair of setscrews opposite each
other to clamp on two opposing flats.

Good luck,
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 ---