I was making those turners' cubes, from 2 inch aluminum blocks
(6061).

I used a 1/4" end mill.

After making about 4 or 5 cubes, the end mill broke.

My question is, how much life expectancy shoudl I expect from a 1/4"
end mill?

Carbide?
HSS?

My parameters are something like

2,000 RPM
6 IPM
Flood coolant (I do not always do a perfect job at directing it, but I
always try and spray it from all directions.

"Ignoramus1419" wrote in message
...
I was making those turners' cubes, from 2 inch aluminum blocks
(6061).

I used a 1/4" end mill.

After making about 4 or 5 cubes, the end mill broke.

My question is, how much life expectancy shoudl I expect from a 1/4"
end mill?

Carbide?
HSS?

My parameters are something like

2,000 RPM
6 IPM
Flood coolant (I do not always do a perfect job at directing it, but I
always try and spray it from all directions.

I am not the person to answer your question, but I wonder if you could sense
when an end mill is about to break by monitoring the stage motor current? I
am presuming it breaks because it gets dull and offers more resistance to
the stage movement increasing the current. Do modern CNC mills have any
feature like this?

Ignoramus1419 wrote:

I was making those turners' cubes, from 2 inch aluminum blocks
(6061).

I used a 1/4" end mill.

After making about 4 or 5 cubes, the end mill broke.

My question is, how much life expectancy shoudl I expect from a 1/4"
end mill?

Carbide?
HSS?

My parameters are something like

2,000 RPM
6 IPM
Flood coolant (I do not always do a perfect job at directing it, but I
always try and spray it from all directions.

It is usually best to remove as much material as possible per rev of the
cutter when roughing. The cubes may need slower cuts as you work inward
due to the minimal support of the inner cubes. But, taking very fine cuts
wears out the cutting edges faster for the amount of metal removed.

I started out with some Stellite cutters, and had no idea they were anything
special. They lasted many years, but eventually got dull, suffered
accidents, etc. When I got some new HSS bits, I was astounded at the short
life, I burned some up in minutes, others lasted a few hours.

Name-brand cutters ARE better. I used to get this flyer with overstock
name-brand (Hanita, Iscar, ITW, etc.) end mills for $3 - 5 each in 1/8 to
3/8" sizes. They eventually started supplying this HORRIBLE Chinese crap in
blue tubes with rubber-stamped labels that looked like they were freehand
sharpened on a bench grinder by a blind 80-year old guy with shaky hands.
Not only was the sharpening bad, the quality of the metal was bad, too.
So, I didn't buy any of that stuff again.

Since then, I have moved largely to M42 HSS with Cobalt in the larger sizes,
and these are MUCH tougher. For 1/8" I use solid carbide, as they are so
cheap.

Also, coolant makes a big difference. I got some TriCool some years ago,
and it was awful. When I got the sample of Encool, it greatly improved the
life of even the plain HSS cutters, about three times! I was very
pleasantly surprised by that!

If you run carbide to where it gets hot, then the coolant can cause thermal
stress fractures and shorten the life of the cutter. 2000 RPM probably is
not getting a 1/4" carbide cutter hot at all. But, it could be getting the
workpiece hot. Often, especially with aluminum, you want to take light cuts
and keep the feedrate way up, maybe 15 - 25 IPM to prevent local heating of
the workpiece.

2000 RPM on a 1/4" end mill is only 130 SFPM, quite slow even for HSS in
aluminum. With a 4-flute end mill at 2000 RPM, this is .00075 inch per
tooth, which is quite low. Normally, for aluminum, a chip load of .010"
per inch of tool diameter is recommended, so that would be .0025 feed per
tooth, or 20 IPM. (Divide by half for a 2-flute cutter.) This is a little
higher than I would normally feed, but I would use 10 IPM for plowing full
width, and probably 15 for half-width.

Jon

"Ignoramus1419" wrote in message
...
I was making those turners' cubes, from 2 inch aluminum blocks
(6061).

I used a 1/4" end mill.

After making about 4 or 5 cubes, the end mill broke.

My question is, how much life expectancy shoudl I expect from a 1/4"
end mill?

Carbide?
HSS?

My parameters are something like

2,000 RPM
6 IPM
Flood coolant (I do not always do a perfect job at directing it, but I
always try and spray it from all directions.

My retired cousin has a CNC Index mill in his home shop and does work for me in return
for materials and tooling. I buy carbide hogging end mills (corn cobs) and "Nachi"
HSS end mills. Nachi mills are preferred for their quality and life. The only thing
is that the job turns into two jobs, roughing and finishing.

My cousin also has little program tips that unload the tool with direction changes and
such to account for the tiny bit of slop in the ball screws. That way the stress on
the tool is minimized. He makes a LOT of parts with that combination of tooling and
programming. He and I use mist cooling satisfactorily.

"Ignoramus1419" wrote in message
...
I was making those turners' cubes, from 2 inch aluminum blocks
(6061).

I used a 1/4" end mill.

After making about 4 or 5 cubes, the end mill broke.

My question is, how much life expectancy shoudl I expect from a 1/4"
end mill?

Carbide?
HSS?

My parameters are something like

2,000 RPM
6 IPM
Flood coolant (I do not always do a perfect job at directing it, but I
always try and spray it from all directions.

Probably you werent flushing out the chips good enough.

In several cases here I routinely cut 6061 for several thousands of hours
running at moderate removal rates using the same hss cutter on horizontals
where ther is plenty of coolant and the chips generally fall freely with no
heat build up in the cut zone.

Sounds like you broke it, not dulled it. Look at the tool, is it dull?
Did you weld AL to it? Did you make it work in a huge pile of
unremoved chips.

I go by feel. You can look at the chips. If they are fine little wispy
things you got too much RPM vs feed.

Use a larger end mill if you possibly can.

With the right cutting conditions, an end mill lasts forever in AL.

Karl

Ignoramus1419 wrote:

I was making those turners' cubes, from 2 inch aluminum blocks
(6061).

I used a 1/4" end mill.

After making about 4 or 5 cubes, the end mill broke.

My question is, how much life expectancy shoudl I expect from a 1/4"
end mill?

Carbide?
HSS?

My parameters are something like

2,000 RPM
6 IPM
Flood coolant (I do not always do a perfect job at directing it, but I
always try and spray it from all directions.

Most likely too low a feed rate again. Possibly dulled, possible chip
welding on the edges. Even with a 1/4" end mill you should be getting
chips coming off that are a good 1/8" wide, not tiny slivers.

Also, what is your depth of cut? Depth of cut mostly relates to spindle
HP requirements, but a 1/4" end mill is relatively small and a high
depth of cut could be causing some deflection and stress.

The width of cut also matters, presuming you're doing a spiral pocket.
The step over needs to be high enough to give a solid cut vs. just rub.
Try 0.10" depth of cut, 0.010 step over and 25 IPM at 2,000 RPM.


Of course it's always possible that a bug in your g-code is giving a
rapid move stress point that the end mill is handling for a while before
failure.

In my manual milling I mostly use HSS end mills, and I rarely break one
that is over 1/16". My go-to AL end mill is a 1/2" two flute high spiral
and that will tear through 6061-T6 AL at ~2,000 RPM and something that
has to be pushing 100 IPM for a side cut of .5" depth x 0.020" width.

Ignoramus1419 wrote in
rec.crafts.metalworking on Mon, 21 Mar 2011 23:47:03 -0500:

Flood coolant (I do not always do a perfect job at directing it, but I
always try and spray it from all directions).

Try aiming it from one side only. Coolant needs to flow across to
carry the chips out. Pockets are a PIA for coolant flow.

--

Dan H.
northshore MA.