I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

Ignoramus5687 wrote:

I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't
your problem, but it's getting you wrapped around the axle and not
focused on where your problem actually is. I machine quite a bit of
aluminum and pretty much never use any sort of coolant, or even sprays
of WD-40. The only time I use fluids on aluminum is when hand tapping.

I can't see your G-code, but forget the coolant and try something like
1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end
mill this is only like 0.005" chip load, very conservative. Watch how it
cuts at that feed rate and try the feed rate override to bump the feed
up if it looks happy. You have a 2-3 HP machine, you should not be
taking cuts that are a fraction of what my 1 HP machine happily takes.

"Pete C." wrote:

Ignoramus5687 wrote:

I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't
your problem, but it's getting you wrapped around the axle and not
focused on where your problem actually is. I machine quite a bit of
aluminum and pretty much never use any sort of coolant, or even sprays
of WD-40. The only time I use fluids on aluminum is when hand tapping.

I can't see your G-code, but forget the coolant and try something like
1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end
mill this is only like 0.005" chip load, very conservative. Watch how it
cuts at that feed rate and try the feed rate override to bump the feed
up if it looks happy. You have a 2-3 HP machine, you should not be
taking cuts that are a fraction of what my 1 HP machine happily takes.

Take a look at: http://wpnet.us/nn_clone/index.htm

Pretty much all of that aluminum was machined dry on my wee little 1J
Bridgeport (except of course for the parts turned dry on my lathe). The
only place coolant was used was on the engraving with a tiny carbide
engraving bit.

On 2010-07-30, Pete C. wrote:

"Pete C." wrote:

Ignoramus5687 wrote:

I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't
your problem, but it's getting you wrapped around the axle and not
focused on where your problem actually is. I machine quite a bit of
aluminum and pretty much never use any sort of coolant, or even sprays
of WD-40. The only time I use fluids on aluminum is when hand tapping.

I can't see your G-code, but forget the coolant and try something like
1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end
mill this is only like 0.005" chip load, very conservative. Watch how it
cuts at that feed rate and try the feed rate override to bump the feed
up if it looks happy. You have a 2-3 HP machine, you should not be
taking cuts that are a fraction of what my 1 HP machine happily takes.

Take a look at: http://wpnet.us/nn_clone/index.htm

Pretty much all of that aluminum was machined dry on my wee little 1J
Bridgeport (except of course for the parts turned dry on my lathe). The
only place coolant was used was on the engraving with a tiny carbide
engraving bit.

Pete, I will try some more. The problem is, one mistake and the
endmill snaps off. I think that I should practice with square end
endmills instead of the ball ends. I have much more of those.

i

Ignoramus18915 wrote:

On 2010-07-30, Pete C. wrote:

"Pete C." wrote:

Ignoramus5687 wrote:

I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't
your problem, but it's getting you wrapped around the axle and not
focused on where your problem actually is. I machine quite a bit of
aluminum and pretty much never use any sort of coolant, or even sprays
of WD-40. The only time I use fluids on aluminum is when hand tapping.

I can't see your G-code, but forget the coolant and try something like
1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end
mill this is only like 0.005" chip load, very conservative. Watch how it
cuts at that feed rate and try the feed rate override to bump the feed
up if it looks happy. You have a 2-3 HP machine, you should not be
taking cuts that are a fraction of what my 1 HP machine happily takes.

Take a look at: http://wpnet.us/nn_clone/index.htm

Pretty much all of that aluminum was machined dry on my wee little 1J
Bridgeport (except of course for the parts turned dry on my lathe). The
only place coolant was used was on the engraving with a tiny carbide
engraving bit.

Pete, I will try some more. The problem is, one mistake and the
endmill snaps off. I think that I should practice with square end
endmills instead of the ball ends. I have much more of those.

i

Practice with HSS end mills, not brittle carbide ones.

Ignoramus18915 wrote:

Pete, I will try some more. The problem is, one mistake and the
endmill snaps off. I think that I should practice with square end
endmills instead of the ball ends. I have much more of those.


I've never used ball end end mills so I'm speculating here.

Can you rough out the cavity with a conventional square end end mill?

Since you piqued my interest about ball nose, I'm looking around a bit. Go read page
28-30+

http://www.ingersoll.com/ictc/ictcpu...e/C-C580-3.pdf


Also read:

http://www.kennametal.com/images/pdf...PCFEVMCQFBYIV0

Do you know the difference between climb milling vs conventional? I prefer climb whenever
the machine can handle it. I usually climb mill on bridgeports with leadscrews and on a
cnc it is the normal way since you don't have backlash to any degree compared to lead
screws.



Wes

On 2010-07-30, Wes wrote:
Ignoramus18915 wrote:

Pete, I will try some more. The problem is, one mistake and the
endmill snaps off. I think that I should practice with square end
endmills instead of the ball ends. I have much more of those.


I've never used ball end end mills so I'm speculating here.

Can you rough out the cavity with a conventional square end end mill?

EXACTLY WHAT i WILL DO

Since you piqued my interest about ball nose, I'm looking around a bit. Go read page
28-30+

http://www.ingersoll.com/ictc/ictcpu...e/C-C580-3.pdf

Very fun stuff.



Also read:

http://www.kennametal.com/images/pdf...PCFEVMCQFBYIV0

nice, just what i need

Do you know the difference between climb milling vs conventional? I prefer climb whenever
the machine can handle it. I usually climb mill on bridgeports with leadscrews and on a
cnc it is the normal way since you don't have backlash to any degree compared to lead
screws.

I am reworking everything nowto use climb.

i

"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

LLoyd

On Jul 29, 6:42*pm, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

LLoyd

I also agree wit no coolant necessary. I do lots of milling on 1/4
tooling plates of 6061. I began with mist coolant, but the mister
leaked, so I stored it in an old plastic waste basket. One day the
janitor spotted it and threw it out. It was in a waste basket, right?
Since then I mill dry with two-flute end mills.

Almost all my work is completely through the plate, so chips are not
usually a problem. In your case, they will be. Can you rig up a shop
vacuum to suck out the chips? That and a 1" chip brush will get the
job done.


Paul

On 2010-07-30, wrote:
On Jul 29, 6:42?pm, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

LLoyd

I also agree wit no coolant necessary. I do lots of milling on 1/4
tooling plates of 6061. I began with mist coolant, but the mister
leaked, so I stored it in an old plastic waste basket. One day the
janitor spotted it and threw it out. It was in a waste basket, right?
Since then I mill dry with two-flute end mills.

Almost all my work is completely through the plate, so chips are not
usually a problem. In your case, they will be. Can you rig up a shop
vacuum to suck out the chips? That and a 1" chip brush will get the
job done.

Yes, I have a vac nearby, I suck chips with it routinely

On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

OK, that's good. I guess I was just spinning the cutter too fast.

i

Ignoramus5687 wrote:

On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

OK, that's good. I guess I was just spinning the cutter too fast.

i

No, it's difficult to spin it too fast really, but the feed rate needs
to be appropriate for the cutter RPM. Again it comes down to the chip
load, i.e. the amount of material removed by each flute of the end mill
each time it rotates around, which is a function of the RPM, feed rate
and number of flutes.

Chances are you were feeding far too slow on that first attempt, which
resulted in very thin chips which stayed in the cut area and got mashed
together gumming everything up. I lost track of where that post was, but
you can certainly calculate what your chip load was for it and I bet it
was 0.001" or less which is far too low.

On Fri, 30 Jul 2010 06:51:20 -0500, "Pete C."
wrote the following:


Ignoramus5687 wrote:

On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

OK, that's good. I guess I was just spinning the cutter too fast.

i

No, it's difficult to spin it too fast really, but the feed rate needs
to be appropriate for the cutter RPM. Again it comes down to the chip
load, i.e. the amount of material removed by each flute of the end mill
each time it rotates around, which is a function of the RPM, feed rate
and number of flutes.

Chances are you were feeding far too slow on that first attempt, which
resulted in very thin chips which stayed in the cut area and got mashed
together gumming everything up. I lost track of where that post was, but
you can certainly calculate what your chip load was for it and I bet it
was 0.001" or less which is far too low.

I haven't yet started machining metal (my jobs are usually minor fab
and in sheet metal), but I think I just tasted a key element in my
education here, Pete. Thanks for sharing that.

--
To see what is right, and not to do it, is want of courage or of principle.
-- Confucius

Ignoramus5687 wrote:

On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

OK, that's good. I guess I was just spinning the cutter too fast.

i

Additionally, note that there are a lot of folks out there cutting
aluminum dry, with a CNC router spinning a bit at 20,000 RPM and moving
at quite high feed rates on home built CNC routers. You can find a bunch
of these online.

On 2010-07-30, Pete C. wrote:

Ignoramus5687 wrote:

On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427
:

but forget the coolant

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete
on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving
significant amounts of metal -- even with my old BP "M" head, which is
fractional HP.

OK, that's good. I guess I was just spinning the cutter too fast.

i

Additionally, note that there are a lot of folks out there cutting
aluminum dry, with a CNC router spinning a bit at 20,000 RPM and moving
at quite high feed rates on home built CNC routers. You can find a bunch
of these online.

I saw a video of that, very impressive.

i

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

Ignoramus5687 wrote:

I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't
your problem, but it's getting you wrapped around the axle and not
focused on where your problem actually is. I machine quite a bit of
aluminum and pretty much never use any sort of coolant, or even sprays
of WD-40. The only time I use fluids on aluminum is when hand tapping.

agree with the above - with the last piece of aluminum I machined on my
Abene mill, I needed a 1/2 inch by 3/4 inch deep rabbet around the edges of
a slab - I put in a 1 inch end mill at whatever my table of RPM said for
aluminum and milled it in a single pass, I think I had the feed set to 4
inches per minute, but it's been a while - worked perfectly. of course this
is a manual mill, not CNC, but that shouldn't matter

"Ignoramus5687" wrote in message
...
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

I had pretty good luck machining aluminum with an end mill made for aluminum
and a mist coolant setup. I think the mist coolant system mainly helped by
blowing chips away from the cutter. My end mill was a 3 flute for aluminum
that I bought from McMaster Carr IIRC. The 3 flutes gave more strength than
2 flute and more chip clearance than a 4 flute, or at least the ad said
something to that effect. It's time to put Quincy to work!

RogerN

On 2010-07-30, RogerN wrote:

"Ignoramus5687" wrote in message
...
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

i

I had pretty good luck machining aluminum with an end mill made for aluminum
and a mist coolant setup. I think the mist coolant system mainly helped by
blowing chips away from the cutter. My end mill was a 3 flute for aluminum
that I bought from McMaster Carr IIRC. The 3 flutes gave more strength than
2 flute and more chip clearance than a 4 flute, or at least the ad said
something to that effect. It's time to put Quincy to work!

Roger, just how far do the chips fly?

i

On 2010-07-30, Ignoramus5687 wrote:
Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

Actually I have decided to make a pump from the mill to work. It is
inside the mill's base. It is not that hard to get to, through the
side door.

I will make the coolant pump controlled by EMC instead of just the
panel switch. That way I will be able to turn on coolant with M8
command.

The weird thing is that there is liquid in the sump now, but it seems
to be straight oil. Once I get it to work, hopefully tonight, I will
pump it all out and look. It may be all the lubricating oil from the
ways that accumulated.

i

Ignoramus5687 wrote:
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

I'm not sure coolant really helps pick up the feedrate. From the other
thread it seems you are
using a 3/8" endmill? I'd probably use 1800 RPM there, and for a
4-flute cutter I'd feed at
about 10 IPM. And, much better to take lighter cuts and keep the cutter
moving rather than taking a deep cut and crawling.
At least, that's MY method.

That oil in your sump is probably an oil-based coolant. Might be even
messier than water-based, but it
probably works fine, too.

Jon

On 2010-07-30, Jon Elson wrote:
Ignoramus5687 wrote:
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

I'm not sure coolant really helps pick up the feedrate. From the other
thread it seems you are
using a 3/8" endmill? I'd probably use 1800 RPM there, and for a
4-flute cutter I'd feed at
about 10 IPM. And, much better to take lighter cuts and keep the cutter
moving rather than taking a deep cut and crawling.
At least, that's MY method.

I think that part of my problem is that I use a ball endmill. I will
mess more with it on the weekend.

That oil in your sump is probably an oil-based coolant. Might be even
messier than water-based, but it
probably works fine, too.


No, it is just a mess of way oil that accumulated.

i

"Ignoramus18915" wrote in message
...
On 2010-07-30, Jon Elson wrote:
Ignoramus5687 wrote:
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

I'm not sure coolant really helps pick up the feedrate. From the other
thread it seems you are
using a 3/8" endmill? I'd probably use 1800 RPM there, and for a
4-flute cutter I'd feed at
about 10 IPM. And, much better to take lighter cuts and keep the cutter
moving rather than taking a deep cut and crawling.
At least, that's MY method.

I think that part of my problem is that I use a ball endmill. I will
mess more with it on the weekend.

It can be difficult to get adequate surface speed near the center of a
ball-nose cutter. It's tricky to program them for complex cuts, and plowing
through solid metal with one is problematic.

You usually use them to get the radius you need when you're cutting only on
one side, and even then, you have to program speeds and feeds carefully so
you aren't pushing the center of the ball at a rate faster than it will
actually cut chips. Profiling is especially tricky.

As for speeds, you can't run an ordinary mill at surface speeds in aluminum
that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn
it too fast for HSS. And that's even running dry.

--
Ed Huntress

On 2010-07-30, Ed Huntress wrote:

"Ignoramus18915" wrote in message
...
On 2010-07-30, Jon Elson wrote:
Ignoramus5687 wrote:
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

I'm not sure coolant really helps pick up the feedrate. From the other
thread it seems you are
using a 3/8" endmill? I'd probably use 1800 RPM there, and for a
4-flute cutter I'd feed at
about 10 IPM. And, much better to take lighter cuts and keep the cutter
moving rather than taking a deep cut and crawling.
At least, that's MY method.

I think that part of my problem is that I use a ball endmill. I will
mess more with it on the weekend.

It can be difficult to get adequate surface speed near the center of a
ball-nose cutter. It's tricky to program them for complex cuts, and plowing
through solid metal with one is problematic.

You usually use them to get the radius you need when you're cutting only on
one side, and even then, you have to program speeds and feeds carefully so
you aren't pushing the center of the ball at a rate faster than it will
actually cut chips. Profiling is especially tricky.

As for speeds, you can't run an ordinary mill at surface speeds in aluminum
that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn
it too fast for HSS. And that's even running dry.

Maybe I should change the whole program. I need to cut out a circular
area of two nested cones:


\__ __/
\___/

Maybe I should get a regular square end mill and mill out two circular
pockets (wider on top and narrower on the bottom). Then change tool to
ball endmill and finish the sides and bottom.

i

"Ignoramus18915" wrote in message
...
On 2010-07-30, Ed Huntress wrote:

"Ignoramus18915" wrote in message
...
On 2010-07-30, Jon Elson wrote:
Ignoramus5687 wrote:
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

I'm not sure coolant really helps pick up the feedrate. From the other
thread it seems you are
using a 3/8" endmill? I'd probably use 1800 RPM there, and for a
4-flute cutter I'd feed at
about 10 IPM. And, much better to take lighter cuts and keep the
cutter
moving rather than taking a deep cut and crawling.
At least, that's MY method.

I think that part of my problem is that I use a ball endmill. I will
mess more with it on the weekend.

It can be difficult to get adequate surface speed near the center of a
ball-nose cutter. It's tricky to program them for complex cuts, and
plowing
through solid metal with one is problematic.

You usually use them to get the radius you need when you're cutting only
on
one side, and even then, you have to program speeds and feeds carefully
so
you aren't pushing the center of the ball at a rate faster than it will
actually cut chips. Profiling is especially tricky.

As for speeds, you can't run an ordinary mill at surface speeds in
aluminum
that are too fast for a carbide cutter. With a 3/8" endmill, you can't
turn
it too fast for HSS. And that's even running dry.

Maybe I should change the whole program. I need to cut out a circular
area of two nested cones:


\__ __/
\___/

Maybe I should get a regular square end mill and mill out two circular
pockets (wider on top and narrower on the bottom). Then change tool to
ball endmill and finish the sides and bottom.

i

That's how it's generally done. If you can find some info on CNC moldmaking,
you'll learn a lot about this kind of job. I haven't checked recently but
some of the CAD and CAM companies have, in the past, had illustrated online
descriptions of their pocketing, profiling, and contouring routines.

If my old articles on the subject were still online, I could point you to a
couple of them. g I covered the subject for _Machining_ and _Machine Shop
Guide_.

That's why I don't want to do CNC at home. It's too close to what I did for
work.

--
Ed Huntress

Ignoramus18915 wrote:

On 2010-07-30, Ed Huntress wrote:

"Ignoramus18915" wrote in message
...
On 2010-07-30, Jon Elson wrote:
Ignoramus5687 wrote:
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports).

This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40.

The good news is that nothing gums up, the bad news is that the speed
is ridiculously slow. Yes, it is CNC, but still.

Next thing on my list is getting coolant to work. I have a
professional coolant tank with motor etc and also a little 1/70 HP
pump that works great in plastic buckets. I think that I will use the
latter Then I can go at the same 1200 RPM but at much higher feeds.

I'm not sure coolant really helps pick up the feedrate. From the other
thread it seems you are
using a 3/8" endmill? I'd probably use 1800 RPM there, and for a
4-flute cutter I'd feed at
about 10 IPM. And, much better to take lighter cuts and keep the cutter
moving rather than taking a deep cut and crawling.
At least, that's MY method.

I think that part of my problem is that I use a ball endmill. I will
mess more with it on the weekend.

It can be difficult to get adequate surface speed near the center of a
ball-nose cutter. It's tricky to program them for complex cuts, and plowing
through solid metal with one is problematic.

You usually use them to get the radius you need when you're cutting only on
one side, and even then, you have to program speeds and feeds carefully so
you aren't pushing the center of the ball at a rate faster than it will
actually cut chips. Profiling is especially tricky.

As for speeds, you can't run an ordinary mill at surface speeds in aluminum
that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn
it too fast for HSS. And that's even running dry.

Maybe I should change the whole program. I need to cut out a circular
area of two nested cones:

\__ __/
\___/

Maybe I should get a regular square end mill and mill out two circular
pockets (wider on top and narrower on the bottom). Then change tool to
ball endmill and finish the sides and bottom.

i

That follows the same concept of using a roughing mill and then a finish
mill.

If you ramp your regular end mill down in small Z steps, say 0.100" and
are at your top 3,000 RPM, you can move at a much higher feed rate, say
30 IPM as a starting point.

Your spindle RPM and the number of flutes on the end mill determines the
feed rate that will give you a reasonable chip load. Your available HP
determines how deep a cut you can take at that chip load.

With your 2-3 HP available, I expect you can take deeper than 0.100"
cuts with ease, but you probably want to limit it to 0.100" cuts to
leave a smaller stairstep for your finish pass. This doesn't mean you
can't optimize things with a roughing and finish pass with the regular
end mill, using a much deeper cut for the initial bulk removal passes,
and a 0.100" step for the final pass with the regular end mill.

Ignoramus18915 wrote:

Maybe I should change the whole program. I need to cut out a circular
area of two nested cones:


\__ __/
\___/

Maybe I should get a regular square end mill and mill out two circular
pockets (wider on top and narrower on the bottom). Then change tool to
ball endmill and finish the sides and bottom.
Yes, that is an excellent plan. There are also bull-nose end mills that
have a radius at the tip, but a flat center. But, you never want to do
roughing with a ball-end mill, due to the center not having any
rotation. It is forced to "churn" the metal instead of cutting it.
This is likely your problem, that churning causes both the work and tool
to run extremely hot. The curved side of the ball-end mill can cut, but
any contact with the center should be avoided.

Jon