I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

fired this volley in
:

all 1 3/8" deep.


How do you figure to get a 1-3/8" deep slot from a cutter that only has a
5/8" cutting depth?

If you take the cuts in shallow increments, AND you don't have any play
in your spindle, you should be able to get within a half-thou. of the
cutter diameter, or so.

But not that depth!

L

On Saturday, January 16, 2016 at 10:20:20 AM UTC-5, Clare wrote:


If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

I think I would do it on a table saw. You could try making one out of wood and see how accurate you can make the slots.

Wear eye protection

Dan

wrote in message
...
I've got a little job I need to do/get done. I am working on the
wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut
end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long,
and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if
I
drilled a row of 1/8" or 5/32 holes down the center of the slot
first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot
easier,
but nobody has them any more.

http://www.mscdirect.com/browse/tn/T...navid=12108552

On Sat, 16 Jan 2016 10:20:28 -0500, wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

I'm going to assume the slot depth is 3/8", not 1-3/8". While the 3/16
end mill may cut close to .188, as measured with a block or pin,
unless you have flood coolant with plenty of velocity available
(unlikely on an un-enclosed mill) the sides of the slot will be quite
rough. I'd use a 5/32 2-flute cutter. Bring the slot to within .010 of
depth with a couple passes with the cutter on center line. Widen the
slot by offsetting the cutter about .005 per side and measure the
result. Set your final offsets taking into account the result of the
previous cut and bring the slot to final depth at the same time. You
can climb mill the final passes if you find you get a better finish
that way. Brush on some alum-tap or kero or WD40 before each pass.

Don't bother with the drilled holes unless the slots have blind ends.
If they do, a hole to depth at each end gives the end mill a place to
dwell at the ends without rubbing, and acts as a visual cue.

Not knowing the condition of the mill it's hard to predict how close
you'll get, but with a bit of care I'd expect to get within 3-5 tenths
on my DRO equipped pretty-tight mill. Within a few thousandths without
paying a lot of attention.

--
Ned Simmons

On 16/01/16 15:20, wrote:
I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.
From those details if you want to do the job I would have thought you
would be better off using an arbor and a slitting saw or side and face
cutter.

On Sat, 16 Jan 2016 10:03:28 -0600, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:

fired this volley in
:

all 1 3/8" deep.


How do you figure to get a 1-3/8" deep slot from a cutter that only has a
5/8" cutting depth?

If you take the cuts in shallow increments, AND you don't have any play
in your spindle, you should be able to get within a half-thou. of the
cutter diameter, or so.

But not that depth!

L
Lay the 1X1 in the vise, with the desired slot vertical. Mill the slot
from the end to the stop-hole. Keep milling bit by bit 'till you
reasch full 5/8" depth for the full 1 3/8" length of the slot. Release
the vise and flip part end to end, reclamp and repeat, cutting from
the other end, untill the depth of cut excedes 3/8" and there is no
more metal in the slot.

On Sat, 16 Jan 2016 10:01:04 -0800 (PST), "
wrote:

On Saturday, January 16, 2016 at 10:20:20 AM UTC-5, Clare wrote:


If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

I think I would do it on a table saw. You could try making one out of wood and see how accurate you can make the slots.

Wear eye protection

Dan
The fun comes in holding the piece in place verticaly, cutting the
slot 1 3/8" deep into the end of the workpiece while dodging all the
flying hot and sharp chips, and getting an acceptable finish AND
accurate slot width.. This needs to be "aircraft precision", not "
lay it out with a crayon and cut with an axe"
These 8 pieces keep the wing from folding up in flight, or falling to
the ground on landing.

On Sat, 16 Jan 2016 13:37:21 -0500, "Jim Wilkins"
wrote:

wrote in message
.. .
I've got a little job I need to do/get done. I am working on the
wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut
end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long,
and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if
I
drilled a row of 1/8" or 5/32 holes down the center of the slot
first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot
easier,
but nobody has them any more.

http://www.mscdirect.com/browse/tn/T...navid=12108552


The cutter would have to be at leadt 2 3/4" plus the diameter of the
arbor to do the job. Unlike an end mill, you can't cut to a straight
end cutting through the 1 inch dimension, and you can't flip it over
to cut from the other end.

I thought about trying to jig the parts up to slit the ends with the
14 inch cutoff saw (abrasive wheel) but the thought of loading the
wheel with aluminum changed my mind on that pretty quick - not to
mention the flexability of the fiber abrasive wheel..

A "cold cut" saw would work - it turns a bit slower than the average
table saw, and the blade is made for cutting metal - but I don't have
one and the quality of the finish of the cut would likely leave
something to be desired.

On Sat, 16 Jan 2016 13:40:12 -0500, Ned Simmons
wrote:

On Sat, 16 Jan 2016 10:20:28 -0500, wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

I'm going to assume the slot depth is 3/8", not 1-3/8". While the 3/16
end mill may cut close to .188, as measured with a block or pin,
unless you have flood coolant with plenty of velocity available
(unlikely on an un-enclosed mill) the sides of the slot will be quite
rough. I'd use a 5/32 2-flute cutter. Bring the slot to within .010 of
depth with a couple passes with the cutter on center line. Widen the
slot by offsetting the cutter about .005 per side and measure the
result. Set your final offsets taking into account the result of the
previous cut and bring the slot to final depth at the same time. You
can climb mill the final passes if you find you get a better finish
that way. Brush on some alum-tap or kero or WD40 before each pass.

Don't bother with the drilled holes unless the slots have blind ends.
If they do, a hole to depth at each end gives the end mill a place to
dwell at the ends without rubbing, and acts as a visual cue.

Not knowing the condition of the mill it's hard to predict how close
you'll get, but with a bit of care I'd expect to get within 3-5 tenths
on my DRO equipped pretty-tight mill. Within a few thousandths without
paying a lot of attention.
The slot depth is the full 1 inch thickness of the stock, and the
length of the slot is 1 3/8"
The mill doesn't have a DRO. It is old but lightly used and well
maintained. Being a 3/8" mill holder, it is almost impossible to buy
an end-mill smaller than 3/16 with a length of 1/2" or more, which is
required to cut the full slot, cutting from both sides. Our local
machine tool supplier doesn't carry them, but an old machinist friend
has a 5/8" long cutter from a box of cutters he bought at a close-out
auction over 10 years ago - brand new never been used, that he has
given me.

On Sat, 16 Jan 2016 14:22:09 -0500, wrote:

On Sat, 16 Jan 2016 13:37:21 -0500, "Jim Wilkins"
wrote:

wrote in message
. ..
I've got a little job I need to do/get done. I am working on the
wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut
end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long,
and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if
I
drilled a row of 1/8" or 5/32 holes down the center of the slot
first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot
easier,
but nobody has them any more.

http://www.mscdirect.com/browse/tn/T...navid=12108552


The cutter would have to be at leadt 2 3/4" plus the diameter of the
arbor to do the job. Unlike an end mill, you can't cut to a straight
end cutting through the 1 inch dimension, and you can't flip it over
to cut from the other end.

I thought about trying to jig the parts up to slit the ends with the
14 inch cutoff saw (abrasive wheel) but the thought of loading the
wheel with aluminum changed my mind on that pretty quick - not to
mention the flexability of the fiber abrasive wheel..

A "cold cut" saw would work - it turns a bit slower than the average
table saw, and the blade is made for cutting metal - but I don't have
one and the quality of the finish of the cut would likely leave
something to be desired.

Cold saws are cutoff saws. With a few exceptions (Amada makes one
such) they don't leave a great finish.

What you want, I think, is someone equipped with a horizontal mill who
does a lot of slotting work. As for the geometry, shank-type cutters
for a vertical mill can cut slots, but I've never seen one that could
handle that depth. Arbor-type slotting mills are the tools that would
give you the accuracy and finish you're talking about, and they're
mostly horizontal-mill tools. They come in a wide range of diameters.

I'm speaking not as one who has done it, but who has seen thousands of
milling cutters and tool setups -- run by other people. d8-)

--
Ed Huntress

On Sat, 16 Jan 2016 18:46:34 +0000, David Billington
wrote:

On 16/01/16 15:20, wrote:
I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.
From those details if you want to do the job I would have thought you
would be better off using an arbor and a slitting saw or side and face
cutter.
If I has an arbour and 3 inch (minimum) cutter that I could mount in
the Myford I could do it, but I'd still have to figure out a way to
square the end of the cut because it would have a 1.5" radius which
may or may not be centered in the piece, depending how I managed to
clamp the piece to the cross-slide. The bigger the cutter, the closer
to straight the end of the cut would be.. Hard to move the part
virtically toclean up the end of the cut.

I just talked to a friend from my highschool years who is a machinist
(usually works a lathe on parts up to 3 1/2 feet in diameter and up
to 20 feet long - both turning the outside and boring) and he said
he'd set up on the "little" cnc mill and do them for me in his spare
time over the next week if I just drop them off for him -
So that's THAT problem solved.!!!

I've done a fair bit of computer stuff for him over the last few
years, so now I'm getting "payback"

On Sat, 16 Jan 2016 10:20:28 -0500, wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

Just make a number of passes. Say 1/8" depth of cut at a time and if
necessary use an air hose to blow the chips out of the cut. Use a
cutting speed and feed rate that doesn't put a great strain on the
tool.

In another message yo talk about this being a part on an airplane.
I've made similar bits for military aircraft this way with no
problems.
--

Cheers,

John B.

On Saturday, January 16, 2016 at 2:22:00 PM UTC-5, Clare wrote:

A "cold cut" saw would work - it turns a bit slower than the average
table saw, and the blade is made for cutting metal - but I don't have
one and the quality of the finish of the cut would likely leave
something to be desired.

You have a solution with your friend doing it. But do not knock using a table saw with carbide tipped teeth for cutting aluminium until you have tried it. It is noisy, but quick. And the finish is not bad. Try searching on " cutting aluminium table saw ". You will get a couple of pages of links to that topic.

Dan

On Sat, 16 Jan 2016 17:07:12 -0800 (PST), "
wrote:

On Saturday, January 16, 2016 at 2:22:00 PM UTC-5, Clare wrote:

A "cold cut" saw would work - it turns a bit slower than the average
table saw, and the blade is made for cutting metal - but I don't have
one and the quality of the finish of the cut would likely leave
something to be desired.

You have a solution with your friend doing it. But do not knock using a table saw with carbide tipped teeth for cutting aluminium until you have tried it. It is noisy, but quick. And the finish is not bad. Try searching on " cutting aluminium table saw ". You will get a couple of pages of links to that topic.

Dan
I've done it several times. I had a 10 inch "Beaver" table saw and
used it to cut 2 inch blocks of aluminum for the engine mounts.(sold
the table saw almost 10 years ago - did I mention we are 16 years into
this build???) The whole garage was full of sharp shiny chips of
aluminum.

I also cut some 3/16" aluminum plate for an engine cover - and that
cost me over $100 for a new armature for my favorite circular saw -and
spread chips all over the back yard. THAT cut was extremely noizy-.

The cuts were smoother than chopping with an axe, but would require a
lot of sanding or grinding to make the surface quality I want for
these parts - which would make any kind of accuracy very difficult.

On 2016-01-16, wrote:
I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

O.K. That 1x1" -- is that square solid stock, or angle stock?

And the 1-3/8" deep suggests that the cuts are from the end, not
through the thickness, even if it is solid square stock.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters,

It should be able to use a number of other different shank
diameters, presuming the availability of collets or end-mill holders in
those sides. Most Bridgeports will use R-8 sized collets or similar
end-mill holders (and the holders have the benefit that the end mill
can't be pulled down into the workpiece as sometimes happens with
collets.

Some (mostly old CNC Bridgeports) use NTMB-30 tool holders
instead, and those also come in a number of sizes.

I'm not sure how common 1/8" end mills with 3/8" shanks will be.
I would expect those to be 1/4" shanks or smaller, though you can
probably get them with large shanks at extra cost.

and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut)

You're going to need a number of passes first off -- and are
limited to the 5/8" depth at best, so how you are going to get 1-3/8"
deep cuts is open to question. If you mean that the slots will be
1-3/8" *long* instead -- that is easier.

In any case -- use something like WD-40 or kerosene as a cutting
lube, and make sure that your end mills are two-flute center cutting
ones. Yes, more flutes remove more material, but for slots, there is a
particular benefit to the two-flute end mills. Yes, the end mill will
deflect during part of the cut -- but that is when one flute is in the
direction of the cut, and the other flute will be in air behind the cut.
A four-flute or more end mill has flutes out to the side during the
deflection while the one in the direction of cut is taking its heaviest
cut, so the sides will show that deflection.

It is for this reason that the UK metalworkers refer to
two-flute end-mills as "slot drills".

Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

It might actually make things worse, as the flutes catch on the
back side of the holes and try to pull the work deeper. If the milling
machine has worn leadscrews and there is backlash this could be a
problem.

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

Not *nobody*. I've got one. So does at least two other
persons that I know semi-locally. (All hobbyists, FWIW.)

Good Luck,
DoN.

--
Remove oil spill source from e-mail
Email: | (KV4PH) 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 17 Jan 2016 02:44:58 GMT, "DoN. Nichols"
wrote:

On 2016-01-16, wrote:
I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

O.K. That 1x1" -- is that square solid stock, or angle stock?

Solid 6061T6

And the 1-3/8" deep suggests that the cuts are from the end, not
through the thickness, even if it is solid square stock.

It is through the thickness, from the end, to make a "fork"

I may have the use of a bridgeport style mill that used 3/8" shank
cutters,

It should be able to use a number of other different shank
diameters, presuming the availability of collets or end-mill holders in
those sides. Most Bridgeports will use R-8 sized collets or similar
end-mill holders (and the holders have the benefit that the end mill
can't be pulled down into the workpiece as sometimes happens with
collets.

Some (mostly old CNC Bridgeports) use NTMB-30 tool holders
instead, and those also come in a number of sizes.

This one only has the 3/8" tool holder - all that has ever been used
on it in over 35 years.

I'm not sure how common 1/8" end mills with 3/8" shanks will be.
I would expect those to be 1/4" shanks or smaller, though you can
probably get them with large shanks at extra cost.

and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut)

You're going to need a number of passes first off -- and are
limited to the 5/8" depth at best, so how you are going to get 1-3/8"
deep cuts is open to question. If you mean that the slots will be
1-3/8" *long* instead -- that is easier.

The cuts are through and through 1 inch, and 1 3/8" long, from the one
end.

In any case -- use something like WD-40 or kerosene as a cutting
lube, and make sure that your end mills are two-flute center cutting
ones.
2 flute center cutting is what I have
Yes, more flutes remove more material, but for slots, there is a
particular benefit to the two-flute end mills. Yes, the end mill will
deflect during part of the cut -- but that is when one flute is in the
direction of the cut, and the other flute will be in air behind the cut.
A four-flute or more end mill has flutes out to the side during the
deflection while the one in the direction of cut is taking its heaviest
cut, so the sides will show that deflection.

It is for this reason that the UK metalworkers refer to
two-flute end-mills as "slot drills".

Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

It might actually make things worse, as the flutes catch on the
back side of the holes and try to pull the work deeper. If the milling
machine has worn leadscrews and there is backlash this could be a
problem.

Or do I just farm it out to a CNC shop??

If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

Not *nobody*. I've got one. So does at least two other
persons that I know semi-locally. (All hobbyists, FWIW.)

Good Luck,
DoN.
The problem is nobody around here seems to have one. The one I know
that used to be around here could only handle 2 inch cutters - not big
enough to do the job (light duty mini hobby tool of some sort) - the
guy that owned it is dead ond gone - no idea what happened to the
tools.

On 2016-01-16, wrote:
On Sat, 16 Jan 2016 13:40:12 -0500, Ned Simmons
wrote:

On Sat, 16 Jan 2016 10:20:28 -0500, wrote:

[ ... ]

The slot depth is the full 1 inch thickness of the stock, and the
length of the slot is 1 3/8"

O.K. Slots cut across the end and 1-3/8" from the end of the
workpiece to the end of the slot.

The mill doesn't have a DRO. It is old but lightly used and well
maintained. Being a 3/8" mill holder, it is almost impossible to buy
an end-mill smaller than 3/16 with a length of 1/2" or more,

There is a reason for short lengths with small diameters. They
tend to break easily when longer.

Now -- you say it is a "Bridgeport type" mill -- and never say
that it is truly a Bridgeport, so I may interpret that as meaning a
vertical spindle mill of unknown size. If it is truly a Bridgeport, or
a clone of the Bridgeport (there have been many), it should accept
alternate end mill holders and not be stuck at 3/8" diameter. End mill
holders or R-8 collets are both options -- and not that expensive to
purchase for your friend if he does not have them.

which is
required to cut the full slot, cutting from both sides. Our local
machine tool supplier doesn't carry them, but an old machinist friend
has a 5/8" long cutter from a box of cutters he bought at a close-out
auction over 10 years ago - brand new never been used, that he has
given me.

You will probably do better with an adaptor arbor to accept
horizontal milling cutters. Typical arbor diameter is 1", though there
are smaller and larger diameter. A 1" arbor had clamping rings 1-1/4"
diameter (and a key to keep the cutter from spinning on the arbor). It
fits into the R-8 socket in the spindle of the mill. This produces a
horizontal cut, so you will need the workpiece sicking out the side of
the vise.

Now -- for 1-3/8" depth of cut, we need to take half the
diameter of the clamping rings (0.625") and add to that at least the
depth of the needed cut (1-3/8") which brings us up to a 2" radius (4"
diameter) thus eliminating the smallest common cutters, which are 3"
diameter. The other size which I normally see is 6" diameter, which
would be plenty for your task.

Good Luck,
DoN.

--
Remove oil spill source from e-mail
Email: | (KV4PH) 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 Saturday, January 16, 2016 at 8:28:02 PM UTC-5, Clare wrote:

I've done it several times. I had a 10 inch "Beaver" table saw and
used it to cut 2 inch blocks of aluminum for the engine mounts.(sold
the table saw almost 10 years ago - did I mention we are 16 years into
this build???) The whole garage was full of sharp shiny chips of
aluminum.

I also cut some 3/16" aluminum plate for an engine cover - and that
cost me over $100 for a new armature for my favorite circular saw -and
spread chips all over the back yard. THAT cut was extremely noizy-.

The cuts were smoother than chopping with an axe, but would require a
lot of sanding or grinding to make the surface quality I want for
these parts - which would make any kind of accuracy very difficult.

I would not recommend a circular saw for aluminium. But do use a table saw whenever it seems like the best way that I have. I have some sheet metal to keep sawdust out of the motor and it works for aluminium chips too. The aluminium chips are a big pain.

If you do not have any aluminium files, I would recommend getting one. The Type A is the best in my opinion. I have a bunch of files from Boeing Surplus, but they do not work as well for good finishes as the Type A I bought many years ago.

Dan

On 17 Jan 2016 03:06:07 GMT, "DoN. Nichols"
wrote:

On 2016-01-16, wrote:
On Sat, 16 Jan 2016 13:40:12 -0500, Ned Simmons
wrote:

On Sat, 16 Jan 2016 10:20:28 -0500, wrote:

[ ... ]

The slot depth is the full 1 inch thickness of the stock, and the
length of the slot is 1 3/8"

O.K. Slots cut across the end and 1-3/8" from the end of the
workpiece to the end of the slot.

The mill doesn't have a DRO. It is old but lightly used and well
maintained. Being a 3/8" mill holder, it is almost impossible to buy
an end-mill smaller than 3/16 with a length of 1/2" or more,

There is a reason for short lengths with small diameters. They
tend to break easily when longer.

Now -- you say it is a "Bridgeport type" mill -- and never say
that it is truly a Bridgeport, so I may interpret that as meaning a
vertical spindle mill of unknown size. If it is truly a Bridgeport, or
a clone of the Bridgeport (there have been many), it should accept
alternate end mill holders and not be stuck at 3/8" diameter. End mill
holders or R-8 collets are both options -- and not that expensive to
purchase for your friend if he does not have them.

And would never use them again. I'm not sure the brand and model of
the mill - but it is european and the owner jokes he bought it from
Noah's grandson.

which is
required to cut the full slot, cutting from both sides. Our local
machine tool supplier doesn't carry them, but an old machinist friend
has a 5/8" long cutter from a box of cutters he bought at a close-out
auction over 10 years ago - brand new never been used, that he has
given me.

You will probably do better with an adaptor arbor to accept
horizontal milling cutters. Typical arbor diameter is 1", though there
are smaller and larger diameter. A 1" arbor had clamping rings 1-1/4"
diameter (and a key to keep the cutter from spinning on the arbor). It
fits into the R-8 socket in the spindle of the mill. This produces a
horizontal cut, so you will need the workpiece sicking out the side of
the vise.

And again, the tooling would likely never be used again - the mill is
in the maintenance shop of a local leather products factory (belts)
and is used to make tooling - I don't think they have added a
"different" tool to it in 30 years - just replaced cutters as they
wore or were damaged. I think all their tooling is Ti coated HSS -
standard and short from 3/16 to about an inch diameter.

Now -- for 1-3/8" depth of cut, we need to take half the
diameter of the clamping rings (0.625") and add to that at least the
depth of the needed cut (1-3/8") which brings us up to a 2" radius (4"
diameter) thus eliminating the smallest common cutters, which are 3"
diameter. The other size which I normally see is 6" diameter, which
would be plenty for your task.

Good Luck,
DoN.
I am aware of that - I stated it would require a cutter of 2 inches
plus the diameter of the arbour if I was going to do it on a
horizontal mill, or on an arbour on my lathe - and the little
horizontal mill that an old aquaintance used to have could only handle
3 inch cutters - he used it for cutting keyways in shafts and
occaisionally making timing belt (toothed belt) sprockets..

wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Don't cut the slot full-width in one pass. Use an end mill smaller than the
desired slot width. Start right down the middle of the slot, and take cuts
running back and forth the length of the slot, going deeper by about 1/2 the
diameter of the cutter each pass, until you break through the bottom. Then,
offset the part a bit, and take one side up to the desired slot dimension.
Then, offset the other way and do the other side. if the machine is tight,
do these cuts in the climb-milling direction, where the feed is with the
rotation of the cutting edge. This gives dramatically better finish in
aluminum. (If the machine is loose, this cutting direction can cause the
work to jump into the cut, so not a good idea.)

This is all MUCH easier with a CNC machine, of course.

Jon

wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.
How do you get a 1 3/8 deep slot in a 1 x 1" piece of stock?

Jon

On Sat, 16 Jan 2016 10:03:28 -0600, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:

fired this volley in
:

all 1 3/8" deep.


How do you figure to get a 1-3/8" deep slot from a cutter that only has a
5/8" cutting depth?

If you take the cuts in shallow increments, AND you don't have any play
in your spindle, you should be able to get within a half-thou. of the
cutter diameter, or so.

But not that depth!

L

Will take very..very..very careful setup and repeated cuts.

Or simply find a used horizontal mill...OR a used shaper. Problem
solved

Gunner

On Sat, 16 Jan 2016 14:15:23 -0500, wrote:

On Sat, 16 Jan 2016 10:01:04 -0800 (PST), "
wrote:

On Saturday, January 16, 2016 at 10:20:20 AM UTC-5, Clare wrote:


If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

I think I would do it on a table saw. You could try making one out of wood and see how accurate you can make the slots.

Wear eye protection

Dan
The fun comes in holding the piece in place verticaly, cutting the
slot 1 3/8" deep into the end of the workpiece while dodging all the
flying hot and sharp chips, and getting an acceptable finish AND
accurate slot width.. This needs to be "aircraft precision", not "
lay it out with a crayon and cut with an axe"
These 8 pieces keep the wing from folding up in flight, or falling to
the ground on landing.

So the bottoms of the slots will be properly radiused?

"Gunner Asch" wrote in message
news
Will take very..very..very careful setup and repeated cuts.

Or simply find a used horizontal mill...OR a used shaper. Problem
solved

Gunner

A dumont push broach will also work.
Been there done it. Still use the jig for
some slotting jobs.

Best Regards
Tom.

wrote in message
...
On 17 Jan 2016 02:44:58 GMT, "DoN. Nichols"

wrote:

On 2016-01-16, wrote:
I've got a little job I need to do/get done. I am working on the
wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut
end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long,
and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 "
slots -
all 1 3/8" deep.

O.K. That 1x1" -- is that square solid stock, or angle stock?

Solid 6061T6

And the 1-3/8" deep suggests that the cuts are from the end, not
through the thickness, even if it is solid square stock.

It is through the thickness, from the end, to make a "fork"


My Clausing 8525 which is half the size of a Bridgeport can cut a full
depth (1-3/8") slot with a 4" slitting saw held in the cheapest of the
MSC arbors I referenced, though I have to make multiple passes because
the 1/2" collet doesn't transmit much torque. The example I have close
at hand is a home made 3/4" steel boring bar slit 1-1/8" deep into the
end, to tighten onto the bit.

It should be easier in aluminum with a new saw instead of the used
ones I cut steel with.
http://www.mscdirect.com/browse/tn/M...navid=12106272

Makita panel saw blades are cheaper and somewhat larger:
http://www.toolbarn.com/makita-a-900...=547 12183694

-jsw

On Sat, 16 Jan 2016 23:39:01 -0600, Jon Elson
wrote:

wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.

I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)

How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????

Don't cut the slot full-width in one pass. Use an end mill smaller than the
desired slot width. Start right down the middle of the slot, and take cuts
running back and forth the length of the slot, going deeper by about 1/2 the
diameter of the cutter each pass, until you break through the bottom. Then,
offset the part a bit, and take one side up to the desired slot dimension.
Then, offset the other way and do the other side. if the machine is tight,
do these cuts in the climb-milling direction, where the feed is with the
rotation of the cutting edge. This gives dramatically better finish in
aluminum. (If the machine is loose, this cutting direction can cause the
work to jump into the cut, so not a good idea.)

This is all MUCH easier with a CNC machine, of course.

Jon
It will be done on the CNC with a small bit. For the old manual mill
there was no bit available smaller than 3/16 long enough to do the
job.

On Sat, 16 Jan 2016 23:41:11 -0600, Jon Elson
wrote:

wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.
How do you get a 1 3/8 deep slot in a 1 x 1" piece of stock?

Jon
Deep if measured from the end. Through if measured from the side.

More accurately, 1 3/8" long

On Sun, 17 Jan 2016 02:45:43 -0800, Gunner Asch
wrote:

On Sat, 16 Jan 2016 10:03:28 -0600, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:

fired this volley in
m:

all 1 3/8" deep.


How do you figure to get a 1-3/8" deep slot from a cutter that only has a
5/8" cutting depth?

If you take the cuts in shallow increments, AND you don't have any play
in your spindle, you should be able to get within a half-thou. of the
cutter diameter, or so.

But not that depth!

L

Will take very..very..very careful setup and repeated cuts.

Or simply find a used horizontal mill...OR a used shaper. Problem
solved

Gunner
Pretty difficuld to do with a shaper to get a clean cut at the base
of the cut (end of the slot) unless cutting across the stock (1 inch
cut) and then to cut 3/16" wide and 1 3/6" deep would be some fun - -
- -

On Sun, 17 Jan 2016 02:46:49 -0800, Gunner Asch
wrote:

On Sat, 16 Jan 2016 14:15:23 -0500, wrote:

On Sat, 16 Jan 2016 10:01:04 -0800 (PST), "
wrote:

On Saturday, January 16, 2016 at 10:20:20 AM UTC-5, Clare wrote:


If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.

I think I would do it on a table saw. You could try making one out of wood and see how accurate you can make the slots.

Wear eye protection

Dan
The fun comes in holding the piece in place verticaly, cutting the
slot 1 3/8" deep into the end of the workpiece while dodging all the
flying hot and sharp chips, and getting an acceptable finish AND
accurate slot width.. This needs to be "aircraft precision", not "
lay it out with a crayon and cut with an axe"
These 8 pieces keep the wing from folding up in flight, or falling to
the ground on landing.

So the bottoms of the slots will be properly radiused?
That is done by the drilled "stop hole" - or by the end mill
finishing the slot - 3/16" slot with 3/32 radius.

On Sun, 17 Jan 2016 08:00:20 -0500, "Jim Wilkins"
wrote:

wrote in message
.. .
On 17 Jan 2016 02:44:58 GMT, "DoN. Nichols"

wrote:

On 2016-01-16, wrote:
I've got a little job I need to do/get done. I am working on the
wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut
end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long,
and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 "
slots -
all 1 3/8" deep.

O.K. That 1x1" -- is that square solid stock, or angle stock?

Solid 6061T6

And the 1-3/8" deep suggests that the cuts are from the end, not
through the thickness, even if it is solid square stock.

It is through the thickness, from the end, to make a "fork"


My Clausing 8525 which is half the size of a Bridgeport can cut a full
depth (1-3/8") slot with a 4" slitting saw held in the cheapest of the
MSC arbors I referenced, though I have to make multiple passes because
the 1/2" collet doesn't transmit much torque. The example I have close
at hand is a home made 3/4" steel boring bar slit 1-1/8" deep into the
end, to tighten onto the bit.

It should be easier in aluminum with a new saw instead of the used
ones I cut steel with.
http://www.mscdirect.com/browse/tn/M...navid=12106272

Makita panel saw blades are cheaper and somewhat larger:
http://www.toolbarn.com/makita-a-900...=547 12183694

-jsw



The MSC #: 73324048 would do the job IF I had an arbor - and it is
almost $90 plus shipping and brokerage - make that over $125
(Canadian) just for the cutter. - plus the cost of the arbor.

The cheapest arbor -MSC #: 08271058 adds another $45 plus shipping
and brokerage. - and then I need a mill that will take the 1/2" shank.
(which I don't have)

No worries - it's all being done on the CNC machine next week - or
whenever the machine is not in use.

fired this volley in
:

Pretty difficuld to do with a shaper to get a clean cut at the base
of the cut (end of the slot) unless cutting across the stock (1 inch
cut) and then to cut 3/16" wide and 1 3/6" deep would be some fun - -

It's pretty difficult to get a clean, well-matched cut when you have to
flip the work and cut a 'half-slot' on each side, too.

If you don't have the capability to cut a slot that deep, likely you
don't have the tools or experience to get the work perfectly-registered
on the flip, either.

Besides, cutting two 'features' on opposite sides of a piece of stock so
they meet in the middle is NOT "milling a slot". It's exactly what I
just described in the prior sentence.

Rule of thumb -- if you don't have the tools or ability, then farm it out
to someone who does!

I'm not an 'experimental' pilot, but I am a pilot. I know somthing about
how planes are put together (yeah, even the structural parts, having
helped A&Ps over many hundreds of hours, just so I'd learn something). I
seriously doubt that a mating feature like that need be as accurate as
you're demanding in order to be robust and safe. If play is problem,
mill the parts for a too-tight fit, and adjust for perfection with hand
tools.

Lloyd

wrote:


It will be done on the CNC with a small bit. For the old manual mill
there was no bit available smaller than 3/16 long enough to do the
job.

If you want, I have a program online that will generate the G-code for this.
See :
http://pico-systems.com/gcode.html

And get the "milling a rectangular pocket" program. I have some more
specific ones for slots with round ends that I have not published.

Jon

On Sat, 16 Jan 2016 23:41:11 -0600, Jon Elson
wrote:

wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.
How do you get a 1 3/8 deep slot in a 1 x 1" piece of stock?

Kinda makes it a thru-slot, dunnit?

--
No greater wrong can ever be done than to put a good man at the mercy
of a bad, while telling him not to defend himself or his fellows;
in no way can the success of evil be made quicker or surer.
--Theodore Roosevelt

On Sun, 17 Jan 2016 16:06:54 -0800, Larry Jaques
wrote:

On Sat, 16 Jan 2016 23:41:11 -0600, Jon Elson
wrote:

wrote:

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.
How do you get a 1 3/8 deep slot in a 1 x 1" piece of stock?

Kinda makes it a thru-slot, dunnit?
Yes it does - picky picky picky --sg

On Sat, 16 Jan 2016 20:28:11 -0500, wrote:

On Sat, 16 Jan 2016 17:07:12 -0800 (PST), "
wrote:

On Saturday, January 16, 2016 at 2:22:00 PM UTC-5, Clare wrote:

A "cold cut" saw would work - it turns a bit slower than the average
table saw, and the blade is made for cutting metal - but I don't have
one and the quality of the finish of the cut would likely leave
something to be desired.

You have a solution with your friend doing it. But do not knock using a table saw with carbide tipped teeth for cutting aluminium until you have tried it. It is noisy, but quick. And the finish is not bad. Try searching on " cutting aluminium table saw ". You will get a couple of pages of links to that topic.

Dan
I've done it several times. I had a 10 inch "Beaver" table saw and
used it to cut 2 inch blocks of aluminum for the engine mounts.(sold
the table saw almost 10 years ago - did I mention we are 16 years into
this build???) The whole garage was full of sharp shiny chips of
aluminum.

I also cut some 3/16" aluminum plate for an engine cover - and that
cost me over $100 for a new armature for my favorite circular saw -and
spread chips all over the back yard. THAT cut was extremely noizy-.

The cuts were smoother than chopping with an axe, but would require a
lot of sanding or grinding to make the surface quality I want for
these parts - which would make any kind of accuracy very difficult.
Not that it is particularly relevant in this application, my favorite
tool for cutting aluminium is my cheap ass band saw ("Simple Simon"
brand from Wilson Brass and Aluminium Foundry in Toronto) with a 4TPI
wood blade. This saw doesn't even come with a rip fence but
modifications have been made.
---

Gerry :-)}
London,Canada

On Sun, 17 Jan 2016 16:26:02 -0500, wrote:

On Sun, 17 Jan 2016 02:45:43 -0800, Gunner Asch
wrote:

On Sat, 16 Jan 2016 10:03:28 -0600, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:

fired this volley in
:

all 1 3/8" deep.


How do you figure to get a 1-3/8" deep slot from a cutter that only has a
5/8" cutting depth?

If you take the cuts in shallow increments, AND you don't have any play
in your spindle, you should be able to get within a half-thou. of the
cutter diameter, or so.

But not that depth!

L

Will take very..very..very careful setup and repeated cuts.

Or simply find a used horizontal mill...OR a used shaper. Problem
solved

Gunner
Pretty difficuld to do with a shaper to get a clean cut at the base
of the cut (end of the slot) unless cutting across the stock (1 inch
cut) and then to cut 3/16" wide and 1 3/6" deep would be some fun - -
- -

Very simple to do. One simply needs a sawhorse to put the end of the
work if its over table size