High speed machining aluminum... An open discussion.

BRIAN.T · Apr 15, 2019

My go to feeds and speeds for roughing aluminum are... Sometimes I push, sometimes not, but this is my starting point.

1/2 3 flute end mill

2020 sfpm ( 15,432 rpm)
.008 chip load (feed 370)
20% step over (.100)
200% axial depth (1.000) max

I was talking to a pretty experienced guy a while back who told me he was regularly at 800 inches per minute. Which got me wondering "what does he know that I don't?"

I've concluded that either he was trying to impress me with some Titan type numbers or his stepover is 10% or less, in which case what's the point? 800 ipm at 10% or 400 @ 20.

So, what is everyone else's go to high speed parameters? Discuss!

Finegrain · Apr 15, 2019

BT30 spindle (not dual-contact)
3/8" or 1/2" 3-flute
16,000 RPM
288 IPM (.006" chipload)
35% stepover
Up to 1" axial for 3/8", 1-1/4" for 1/2"

I'm very happy with these parameters. Roughing is usually only like 10% of my cycle times so I spend a lot more time optimizing and tuning elsewhere.

Regards.

Mike

BRIAN.T · Apr 15, 2019

Finegrain said:
BT30 spindle (not dual-contact)
3/8" or 1/2" 3-flute
16,000 RPM
288 IPM (.006" chipload)
35% stepover
Up to 1" axial for 3/8", 1-1/4" for 1/2"

I'm very happy with these parameters. Roughing is usually only like 10% of my cycle times so I spend a lot more time optimizing and tuning elsewhere.

Regards.

Mike

That's great, and those are wildly different numbers then mine. I knew this would be interesting. Thanks

DavidScott · Apr 15, 2019

Depends on what you are roughing with. Corncob mills will put you in a different state as far as chip loads go. 3/8" mills are .01"- .035" per tooth, and those are just for starters. Almost always I can't hold onto my parts well enough to even start to push the endmill, bummer.

Matt@RFR · Apr 15, 2019

One can program 370 or 800 inches per minute, but does one actually receive what one asked for? One thinks likely not.

Hazzert · Apr 16, 2019

Matt@RFR said:
One can program 370 or 800 inches per minute, but does one actually receive what one asked for? One thinks likely not.

They sure do if the guy runs it in dry run. I’ve solved that problem for my guys more than once :eek:

gkoenig · Apr 16, 2019

exkenna · Apr 16, 2019

BRIAN.T said:
My go to feeds and speeds for roughing aluminum are... Sometimes I push, sometimes not, but this is my starting point.

1/2 3 flute end mill

2020 sfpm ( 15,432 rpm)
.008 chip load (feed 370)
20% step over (.100)
200% axial depth (1.000) max

I was talking to a pretty experienced guy a while back who told me he was regularly at 800 inches per minute. Which got me wondering "what does he know that I don't?"

I've concluded that either he was trying to impress me with some Titan type numbers or his stepover is 10% or less, in which case what's the point? 800 ipm at 10% or 400 @ 20.

So, what is everyone else's go to high speed parameters? Discuss!

So many variables.. tool, spindle, fixturing, etc. I think your numbers are just fine.
If your spindle is happy and the part stays in the vise all is good.
The real question: Are you making good money at these parameters? If so, you're golden.

BRIAN.T · Apr 16, 2019

Hazzert said:
They sure do if the guy runs it in dry run. I’ve solved that problem for my guys more than once

I'm sure he is referring to the machines ability to accelerate.

Matt@RFR said:
One can program 370 or 800 inches per minute, but does one actually receive what one asked for? One thinks likely not.

As for acc/Dec my 3 axis mills (which are all the same) have a Max feed rate of 370, which I have no problem achieving with the correct Gcode. Without the high speed codes in place the mills only get up to about 200ipm. My 5 axis tops out at about 1200ipm. I've never tried anything above about 500ipm. But ide be inclined to agree that people who program at outrageous feeds rarely see those numbers in practice.

BRIAN.T · Apr 16, 2019

exkenna said:
So many variables.. tool, spindle, fixturing, etc. I think your numbers are just fine.
If your spindle is happy and the part stays in the vise all is good.
The real question: Are you making good money at these parameters? If so, you're golden.

Yeah you are absolutely right. My cat40 (single contact...? Is that the opposite of dual contact) don't always love those numbers. My HSK spindle, sounds like I'm cutting air. Hsk is a beautiful thing.

BRIAN.T · Apr 16, 2019

gkoenig said:

Ahhhhhb so good! Thanks man! Shit made my day.

Speedie · Apr 16, 2019

20 percent is aggressive but that chipload is light. .010 to .015 with a 15 to 18 percent stepover. If the material is held rigidly I dont think your numbers are too far off. If you have the drawbar force and taper for it double that chip load. Most aluminums are just butter needing to be peeled off

Mike1974 · Apr 16, 2019

DavidScott said:
Depends on what you are roughing with. Corncob mills will put you in a different state as far as chip loads go. 3/8" mills are .01"- .035" per tooth, and those are just for starters. Almost always I can't hold onto my parts well enough to even start to push the endmill, bummer.

That is my problem. We do sooo much variety, but most of it ends up being held onto .05" in standard vise jaws. Yes, I know there are better ways to hold onto minimal stock, but we don't have it. Also, as someone else said, roughing is normally (for us anyways) about 5-10% of the time so I don;t see the point in pushing the rough balls out... I know there are other factors, but a big run for us would be 50 pieces too.

dandrummerman21 · Apr 16, 2019

Mike1974 said:
That is my problem. We do sooo much variety, but most of it ends up being held onto .05" in standard vise jaws. Yes, I know there are better ways to hold onto minimal stock, but we don't have it. Also, as someone else said, roughing is normally (for us anyways) about 5-10% of the time so I don;t see the point in pushing the rough balls out... I know there are other factors, but a big run for us would be 50 pieces too.

I often have the same problem. And for most jobs, that is enough, don't try to hog it out super fast, and that is enough.

For slightly better protection, when running steel only holding onto that much, I go with the talon grip jaws that bite in a bit. It is an obvious improvement, but also obviously only works if you are milling all around the part and can flip it.

But lately, I am beginning to consider making my own dovetail soft jaws for those really pesky jobs that i only have a bit to hold onto and need a lot sticking out of the vise. I have a dovetail cutter and some dovetail jaws for the 5th axis vise, and because I see how securely those dovetails hold onto the part, I have a 3axis job on my desk here that I'm gonna dovetail first, because we had pullout issues on it before.

As for speeds and feeds in aluminum, I only have 6000rpm on most machines, so for roughing applications, 6000rpm/150ipm/.25"stepover/1" deep.. I drop to 5000rpm/60ipm/.5" deep for full slotting applications, 1/2" endmill in 7075

I am not breaking any records by any means, but gets the job done quick.

BRIAN.T · Apr 16, 2019

Speedie said:
20 percent is aggressive but that chipload is light. .010 to .015 with a 15 to 18 percent stepover. If the material is held rigidly I dont think your numbers are too far off. If you have the drawbar force and taper for it double that chip load. Most aluminums are just butter needing to be peeled off

That is fascinating, you're approach is backwards from mine, though I definitely love the idea of less stepover with a larger chip, but again on my 3 axis I'm limited with my feeds. Im going to see what kind of chip.i can make on my 5 axis soon. Thanks.

BRIAN.T · Apr 16, 2019

dandrummerman21 said:
6000rpm/300ipm/.25"stepover/1" deep..

I am not breaking any records by any means, but gets the job done quick.

Don't sell yourself short, that's a hell of a chip you're making. Is this cat40?

BRIAN.T · Apr 16, 2019

Mike1974 said:
That is my problem. We do sooo much variety, but most of it ends up being held onto .05" in standard vise jaws. Yes, I know there are better ways to hold onto minimal stock, but we don't have it. Also, as someone else said, roughing is normally (for us anyways) about 5-10% of the time so I don;t see the point in pushing the rough balls out... I know there are other factors, but a big run for us would be 50 pieces too.

It took me about 2 years to convince the owner that more stock was well worth the extra money. Faster roughing, faster setups, far less error. When I started here we (they) would saw cut most parts to size then try to machine precision parts. It was embarrassing.

dstryr · Apr 16, 2019

BRIAN.T said:
My go to feeds and speeds for roughing aluminum are... Sometimes I push, sometimes not, but this is my starting point.

1/2 3 flute end mill

2020 sfpm ( 15,432 rpm)
.008 chip load (feed 370)
20% step over (.100)
200% axial depth (1.000) max

I was talking to a pretty experienced guy a while back who told me he was regularly at 800 inches per minute. Which got me wondering "what does he know that I don't?"

I've concluded that either he was trying to impress me with some Titan type numbers or his stepover is 10% or less, in which case what's the point? 800 ipm at 10% or 400 @ 20.

So, what is everyone else's go to high speed parameters? Discuss!

I'd say your biggest improvements will be from increasing stepover by 5% increments until you find the limit. I have machines with 50hp but roughing tends to be such a small percentage of the overall cycle time for us most of the time. I usually find way more cycle time improvement by running multiple parts a cycle, reducing air cutting, moving to 4/5 flute aluminum finishing cutters. Only takes one chucked part or one broken tool to wipe out the savings of pushing away from process reliability and then it was all for nothing unless you are like Tony or Greg trying to run 10k parts a week and pushing for seconds in saving

Mike1974 · Apr 16, 2019

BRIAN.T said:
It took me about 2 years to convince the owner that more stock was well worth the extra money. Faster roughing, faster setups, far less error. When I started here we (they) would saw cut most parts to size then try to machine precision parts. It was embarrassing.

I tried to 'sell' talon grips here...

Oh well, it appears the agreement is 'fast enough' for roughing when it is such a small part of the machining process. With the odd standouts making a bazillion parts a year.

DavidScott · Apr 16, 2019

I am doing more and more aluminum plates that have to be machined on all surfaces but I get to put a radius on the top, my design. This allows me to reduce the wasted material to a bare minimum but I only get to hold onto .03" to .05" of the part. I despise any waste and the quantities are in the thousands a year so any savings will add up, my designs so as long as they sell I will be making them. It's been a long time coming but I just made a small batch of steel wedge clamps and stops with teeth .015" apart to use in my fixtures. I have found that I only need to bite into the aluminum about .001"-.002" for it to hold. The difference between a smooth clamping surface and one with teeth is AMAZING!!!! So nice to go from babying the thing for fear the parts will pull out of the fixture to not giving it a thought cause they are not going to move, period!

High speed machining aluminum... An open discussion.

Cast Iron

Diamond

Cast Iron

Diamond

Titanium

Stainless

Titanium

Stainless

Cast Iron

Cast Iron

Cast Iron

Stainless

Diamond

Stainless

Cast Iron

Cast Iron

Cast Iron

Diamond

Diamond

Diamond

Similar threads