Thanks to Pete C's advice, I am milling aluminum with HSS end mills.
These are Interstate end mills that Enco sells for $2.99 a piece.

I have to say that they work nicely, at 12 IPM, 2000 RPM, 2 flute,
1/4" diameter of end mill.

I am making those aluminum turner's cubes, which is a process that I
automated, so it takes me no time. All my friends want them.

Right now I am using depth of cut that is 1/3 of the end mill
diameter, and I am wondering if perhaps I am short changing
myself. Can I use depth of cut that is 1/2 of diameter? 1 diameter?
This process involves both slotting, as well as side milling.

i

"Ignoramus30421" wrote in message
...
Thanks to Pete C's advice, I am milling aluminum with HSS end mills.
These are Interstate end mills that Enco sells for $2.99 a piece.

I have to say that they work nicely, at 12 IPM, 2000 RPM, 2 flute,
1/4" diameter of end mill.

I am making those aluminum turner's cubes, which is a process that I
automated, so it takes me no time. All my friends want them.

Right now I am using depth of cut that is 1/3 of the end mill
diameter, and I am wondering if perhaps I am short changing
myself. Can I use depth of cut that is 1/2 of diameter? 1 diameter?
This process involves both slotting, as well as side milling.


http://www.archive.org/download/tuco...nsultant20.zip

--

On Fri, 8 Apr 2011 20:13:13 -0700, "PrecisionmachinisT"
wrote:


"Ignoramus30421" wrote in message
m...
Thanks to Pete C's advice, I am milling aluminum with HSS end mills.
These are Interstate end mills that Enco sells for $2.99 a piece.

I have to say that they work nicely, at 12 IPM, 2000 RPM, 2 flute,
1/4" diameter of end mill.

I am making those aluminum turner's cubes, which is a process that I
automated, so it takes me no time. All my friends want them.

Right now I am using depth of cut that is 1/3 of the end mill
diameter, and I am wondering if perhaps I am short changing
myself. Can I use depth of cut that is 1/2 of diameter? 1 diameter?
This process involves both slotting, as well as side milling.


http://www.archive.org/download/tuco...nsultant20.zip

--


Nice calculator. I hadn't seen this before. The speed feed DOC are way
off the chart compared to what I do. I see it says up to .375 on a .25
EM. I'd be unlikely to try it on a full slot where you're cutting both
sides. But for $3, why not? No guts no glory. They may be assuming
high pressure flood coolant to keep the chips cleared. Something you
don't have.

I see the speed feed are both about 1/3 of what you are running. About
right on a small non production mill, IMHO.


Back to DOC. I've thought the ease of breaking an endmill must vary
with the square of diameter. Or put simply, a 1/16 breaks if you look
at it cross eyed, I only go maybe 10 thou or a fraction of a diameter.
AND only use it when nothing else will do. A 1/4 still breaks easily,
I'd be cautious at one diameter. Go up to 1/2 and you can cut real
deep - 2 diameters wouldn't cause fear.

I've not seen the above in calculators. So, its just one guy's
experience. It may be related to chip removal on my hobby quality
equipment.

Keep in mind, I'm not like Pete. I've broke a lot of end mills.

Karl

On 2011-04-09, Karl Townsend wrote:
On Fri, 8 Apr 2011 20:13:13 -0700, "PrecisionmachinisT"
wrote:


"Ignoramus30421" wrote in message
om...
Thanks to Pete C's advice, I am milling aluminum with HSS end mills.
These are Interstate end mills that Enco sells for $2.99 a piece.

I have to say that they work nicely, at 12 IPM, 2000 RPM, 2 flute,
1/4" diameter of end mill.

I am making those aluminum turner's cubes, which is a process that I
automated, so it takes me no time. All my friends want them.

Right now I am using depth of cut that is 1/3 of the end mill
diameter, and I am wondering if perhaps I am short changing
myself. Can I use depth of cut that is 1/2 of diameter? 1 diameter?
This process involves both slotting, as well as side milling.


http://www.archive.org/download/tuco...nsultant20.zip


Nice calculator. I hadn't seen this before. The speed feed DOC are way
off the chart compared to what I do. I see it says up to .375 on a .25
EM. I'd be unlikely to try it on a full slot where you're cutting both
sides. But for $3, why not? No guts no glory. They may be assuming
high pressure flood coolant to keep the chips cleared. Something you
don't have.

I see the speed feed are both about 1/3 of what you are running. About
right on a small non production mill, IMHO.


Back to DOC. I've thought the ease of breaking an endmill must vary
with the square of diameter. Or put simply, a 1/16 breaks if you look
at it cross eyed, I only go maybe 10 thou or a fraction of a diameter.
AND only use it when nothing else will do. A 1/4 still breaks easily,
I'd be cautious at one diameter. Go up to 1/2 and you can cut real
deep - 2 diameters wouldn't cause fear.

I've not seen the above in calculators. So, its just one guy's
experience. It may be related to chip removal on my hobby quality
equipment.

Keep in mind, I'm not like Pete. I've broke a lot of end mills.

Karl

Yes, I will use at 1/2 diameter.

i

Karl Townsend wrote:

On Fri, 8 Apr 2011 20:13:13 -0700, "PrecisionmachinisT"
wrote:


"Ignoramus30421" wrote in message
m...
Thanks to Pete C's advice, I am milling aluminum with HSS end mills.
These are Interstate end mills that Enco sells for $2.99 a piece.

I have to say that they work nicely, at 12 IPM, 2000 RPM, 2 flute,
1/4" diameter of end mill.

I am making those aluminum turner's cubes, which is a process that I
automated, so it takes me no time. All my friends want them.

Right now I am using depth of cut that is 1/3 of the end mill
diameter, and I am wondering if perhaps I am short changing
myself. Can I use depth of cut that is 1/2 of diameter? 1 diameter?
This process involves both slotting, as well as side milling.


http://www.archive.org/download/tuco...nsultant20.zip

--


Nice calculator. I hadn't seen this before. The speed feed DOC are way
off the chart compared to what I do. I see it says up to .375 on a .25
EM. I'd be unlikely to try it on a full slot where you're cutting both
sides. But for $3, why not? No guts no glory. They may be assuming
high pressure flood coolant to keep the chips cleared. Something you
don't have.

I see the speed feed are both about 1/3 of what you are running. About
right on a small non production mill, IMHO.

Back to DOC. I've thought the ease of breaking an endmill must vary
with the square of diameter. Or put simply, a 1/16 breaks if you look
at it cross eyed, I only go maybe 10 thou or a fraction of a diameter.
AND only use it when nothing else will do. A 1/4 still breaks easily,
I'd be cautious at one diameter. Go up to 1/2 and you can cut real
deep - 2 diameters wouldn't cause fear.

I've not seen the above in calculators. So, its just one guy's
experience. It may be related to chip removal on my hobby quality
equipment.

Keep in mind, I'm not like Pete. I've broke a lot of end mills.

Karl

There are a lot of variables that all interact, I haven't had a chance
to look at the calculator noted, but I expect there are some high end
packages that take all variables into account.

Some thoughts:

- The length of cut, i.e. the amount of material the end mill flute will
sweep through determines the chip size and needs to fit in the available
clearance of the end mill. For slotting the length of cut is the full
dia of the end mill.

- The depth of cut, i.e. how deep the end mill is cutting in the
material on each pass is a function of the length of cut and the
rigidity of the end mill.

If you are slotting, i.e. cutting the full diameter of the end mill, the
dept of the cut is going to be limited by the lesser of machine HP or
end mill rigidity, and to a limited extent the ability of the coolant to
flush the chips out of the way. Recommendation, start testing with a
shallow depth of cut and progressively work to deeper cuts while
monitoring until you can tell that it's starting to stress things, then
back off a bit and use that as your depth of cut.

If you are side milling, the shorter the length of cut (step over), the
longer the depth of cut (step down) you will be able to get away with.

"Pete C." wrote in message
ter.com...

Karl Townsend wrote:

On Fri, 8 Apr 2011 20:13:13 -0700, "PrecisionmachinisT"
wrote:


"Ignoramus30421" wrote in message
m...
Thanks to Pete C's advice, I am milling aluminum with HSS end mills.
These are Interstate end mills that Enco sells for $2.99 a piece.

I have to say that they work nicely, at 12 IPM, 2000 RPM, 2 flute,
1/4" diameter of end mill.

I am making those aluminum turner's cubes, which is a process that I
automated, so it takes me no time. All my friends want them.

Right now I am using depth of cut that is 1/3 of the end mill
diameter, and I am wondering if perhaps I am short changing
myself. Can I use depth of cut that is 1/2 of diameter? 1 diameter?
This process involves both slotting, as well as side milling.


http://www.archive.org/download/tuco...nsultant20.zip

--


Nice calculator. I hadn't seen this before. The speed feed DOC are way
off the chart compared to what I do. I see it says up to .375 on a .25
EM. I'd be unlikely to try it on a full slot where you're cutting both
sides. But for $3, why not? No guts no glory. They may be assuming
high pressure flood coolant to keep the chips cleared. Something you
don't have.

I see the speed feed are both about 1/3 of what you are running. About
right on a small non production mill, IMHO.

Back to DOC. I've thought the ease of breaking an endmill must vary
with the square of diameter. Or put simply, a 1/16 breaks if you look
at it cross eyed, I only go maybe 10 thou or a fraction of a diameter.
AND only use it when nothing else will do. A 1/4 still breaks easily,
I'd be cautious at one diameter. Go up to 1/2 and you can cut real
deep - 2 diameters wouldn't cause fear.

I've not seen the above in calculators. So, its just one guy's
experience. It may be related to chip removal on my hobby quality
equipment.

Keep in mind, I'm not like Pete. I've broke a lot of end mills.

Karl

There are a lot of variables that all interact, I haven't had a chance
to look at the calculator noted, but I expect there are some high end
packages that take all variables into account.

Some thoughts:

- The length of cut, i.e. the amount of material the end mill flute will
sweep through determines the chip size and needs to fit in the available
clearance of the end mill. For slotting the length of cut is the full
dia of the end mill.

- The depth of cut, i.e. how deep the end mill is cutting in the
material on each pass is a function of the length of cut and the
rigidity of the end mill.

If you are slotting, i.e. cutting the full diameter of the end mill, the
dept of the cut is going to be limited by the lesser of machine HP or
end mill rigidity, and to a limited extent the ability of the coolant to
flush the chips out of the way. Recommendation, start testing with a
shallow depth of cut and progressively work to deeper cuts while
monitoring until you can tell that it's starting to stress things, then
back off a bit and use that as your depth of cut.

If you are side milling, the shorter the length of cut (step over), the
longer the depth of cut (step down) you will be able to get away with.

The calculator allows user input of depth /dia. ratio and adjusts the sfm
and chipload output so as to compensate for transverse rupture.

--

PrecisionmachinisT wrote:
(...)

http://www.archive.org/download/tuco...nsultant20.zip

Wow! Really nice!
And it runs great under Linux Wine!

Thanks PM!

--Winston

"Winston" wrote in message
...
PrecisionmachinisT wrote:
(...)

http://www.archive.org/download/tuco...nsultant20.zip

Wow! Really nice!
And it runs great under Linux Wine!

Thanks PM!


Actually, thank Michael Rainey...

--better yet, send him some money or purchase from him a newer version, and/
or one of his other apps

PrecisionmachinisT wrote:
wrote in message
...
PrecisionmachinisT wrote:
(...)

http://www.archive.org/download/tuco...nsultant20.zip

Wow! Really nice!
And it runs great under Linux Wine!

Thanks PM!


Actually, thank Michael Rainey...

--better yet, send him some money or purchase from him a newer version, and/
or one of his other apps

Good idea. I just bought him lunch. Thanks!

--Winston

On 2011-04-09, Winston wrote:
PrecisionmachinisT wrote:
wrote in message
...
PrecisionmachinisT wrote:
(...)

http://www.archive.org/download/tuco...nsultant20.zip

Wow! Really nice!
And it runs great under Linux Wine!

Thanks PM!


Actually, thank Michael Rainey...

--better yet, send him some money or purchase from him a newer version, and/
or one of his other apps

Good idea. I just bought him lunch. Thanks!

--Winston

Works great under WINE, indeed!

i

On Sat, 09 Apr 2011 05:49:42 -0500, Karl Townsend
wrote:

On Fri, 8 Apr 2011 20:13:13 -0700, "PrecisionmachinisT"
wrote:


"Ignoramus30421" wrote in message
om...
Thanks to Pete C's advice, I am milling aluminum with HSS end mills.
These are Interstate end mills that Enco sells for $2.99 a piece.

I have to say that they work nicely, at 12 IPM, 2000 RPM, 2 flute,
1/4" diameter of end mill.

I am making those aluminum turner's cubes, which is a process that I
automated, so it takes me no time. All my friends want them.

Right now I am using depth of cut that is 1/3 of the end mill
diameter, and I am wondering if perhaps I am short changing
myself. Can I use depth of cut that is 1/2 of diameter? 1 diameter?
This process involves both slotting, as well as side milling.


http://www.archive.org/download/tuco...nsultant20.zip

--


Nice calculator. I hadn't seen this before. The speed feed DOC are way
off the chart compared to what I do. I see it says up to .375 on a .25
EM. I'd be unlikely to try it on a full slot where you're cutting both
sides. But for $3, why not? No guts no glory. They may be assuming
high pressure flood coolant to keep the chips cleared. Something you
don't have.

I see the speed feed are both about 1/3 of what you are running. About
right on a small non production mill, IMHO.


Back to DOC. I've thought the ease of breaking an endmill must vary
with the square of diameter. Or put simply, a 1/16 breaks if you look
at it cross eyed, I only go maybe 10 thou or a fraction of a diameter.
AND only use it when nothing else will do. A 1/4 still breaks easily,
I'd be cautious at one diameter. Go up to 1/2 and you can cut real
deep - 2 diameters wouldn't cause fear.

I've not seen the above in calculators. So, its just one guy's
experience. It may be related to chip removal on my hobby quality
equipment.

Keep in mind, I'm not like Pete. I've broke a lot of end mills.

Karl

anyone have a suggestion for a free..or nearly free similar calculator
that will run on an Android cell phone?

I had one that ran very nicely on a PDA...but the PDA finally died and
it never got replaced.

Gunner

--

"You can have peace. Or you can have freedom. Don't ever count on having both at once."
Robert A. Heinlein

OK, my general rules are to use about 1/2 the diameter as the "plunge"
depth, and maybe 1/4 the diameter as the step-over. I reduce the
feed when "plowing" the tool at the full width, as the first pass at this
depth, then pick up the feed on additional passes at that depth.
Feed is calculated by RPM x number of flutes x diameter of end mill.
So, for 2800 RPM x 4 flute x .25" diameter x .010", you get 28 IPM.
(The .010 comes from my McDonnell-Douglas slide rule that gives .010"
for a 1" end mill in Aluminum, and says to multiply feedrate by tool
diameter.)

These numbers may be upper limits, and you need to reduce them when the
workpiece is delicate or not rigidly fixtured. I generally reduce the feed
when plowing to 1/2 to 1/3rd of the feeds calculated by the above method.

Jon

If they were able to do it in ww2 then you can do it too. Multiply your diameter by .003 or .03% and get rid of chatter by slowing down your rpms and you can go 4x the diameter through steel using hss or carbide. Chip loads will make you faster not rpms. I have proof .03% work great when I cut through a 303 stainless bar .750 deep in one shot with a carbide 2 flute. Just remember the constant of .02% of you diameter for hard to cut conditions and 1% for very easy to cut conditions use this for any size tool and keep it under the recomendé sfm or lowere if it chatters. Get rid of chatter even if you have to spin that spindle by hand.

Love that comment you gave about multiplying the tool diameter by .01 to get the chip load for a 1€� endmill. I am right now campaigning this very concept on Facebook bc i feel all the new guys should learn this. Feeds and speeds were so hard for me to learn and practically within the year I got really good at cutting steels and aluminum with the craziest depths and slotting. I noticed the chip load was directly proportional to the diameter of he tool. But for slotting full depth at 3x the diameter of the tool I recommend .002 instead of .01 I got by difficulty of the cut bc people have different concepts of materials. Some say 303stainless is soft. It is but I wouldnt call it soft. And .01 is for easy to cut materials like cast iron and aluminum and plastic
Wow really cool. Im gonna look for that chart you have