One endmill great surface finish in slotting 6061 Question

plutoniumsalmon · Jul 24, 2017

Hello.
When we cut 6061 we usually cut HSM 10 percent stepover and then finish by taking .005 of slowly at full depth (provided its not to deep). I now have bunch of parts that I want to cut as fast as possible and yet keep a decent wall finish. Can I do it in one pass? Slot and leave kind of thing. The details are an open ended slot the doc is .25 and the endmill is 3fl .375. What would be a decent feed and speed for this.

Thank you.

Milland · Jul 24, 2017

For speed, max it out, unless you're running a 50K spindle it's unlikely you can go too fast. For feed, what's your acceptable cusp height? What's your chip handling method, flood coolant? Can you evacuate the slot to prevent loading the endmill?

And what endmill? All three flutes are not alike. Coating, grind, stub or regular length (I'd use a stub here)? How are you holding it, and how many parts will it cut before replacement?

Tl;dr: need more info...

Fadriver · Jul 24, 2017

plutoniumsalmon said:
Hello.
When we cut 6061 we usually cut HSM 10 percent stepover and then finish by taking .005 of slowly at full depth (provided its not to deep). I now have bunch of parts that I want to cut as fast as possible and yet keep a decent wall finish. Can I do it in one pass? Slot and leave kind of thing. The details are an open ended slot the doc is .25 and the endmill is 3fl .375. What would be a decent feed and speed for this.

Thank you.

Don't like 3 flt.
I do 100% aluminum 6061-T6 ,for me 2 flt. about from 3400 to 4200 rpm and about 25 ipm.
the only 3 flute that use is hanita roughers the rest 2 flt.

Milland · Jul 24, 2017

Fadriver said:
Don't like 3 flt.
I do 100% aluminum 6061-T6 ,for me 2 flt. about from 3400 to 4200 rpm and about 25 ipm.
the only 3 flute that use is hanita roughers the rest 2 flt.

Hmm - I was an early adopter of three flute EM's back in the old days when C2 was the carbide of choice. Not sure why you don't like it, but to each their own.

I'm a little surprised nobody's come out with a four flute optimized for Al, I bet it could be done with the right helix angle and aggressive geometry to make it sing...

gkoenig · Jul 24, 2017

Fadriver said:
Don't like 3 flt.
I do 100% aluminum 6061-T6 ,for me 2 flt. about from 3400 to 4200 rpm and about 25 ipm.
the only 3 flute that use is hanita roughers the rest 2 flt.

That's the modern aluminum machining equivalent of this car:

Ideally, you would use two tools; an aluminum rougher (Destiny Diamondback, SwiftCarb RampMill, Frasia X-Gen, Helical) to slot at the full .25" depth at about 100IPM. Finish with a 1/4" 5 flute SwiftCarb finisher on the walls.

If I had to use one tool? I would hit it with a Helical 45 degree helix with a full slot cut and finishing passes (they make a nice one with a .5" LOC so you can keep everything as stubby and rigid as possible).

Keep your flood coolant well managed.

triumph406 · Jul 24, 2017

Fadriver said:
Don't like 3 flt.
I do 100% aluminum 6061-T6 ,for me 2 flt. about from 3400 to 4200 rpm and about 25 ipm.
the only 3 flute that use is hanita roughers the rest 2 flt.

Not sure what machine you have but 25ipm is not exactly pushing the limits. Get a machine that can run 6061 faster (150ipm+) and you'll get to like 3 flute em's

triumph406 · Jul 24, 2017

plutoniumsalmon said:
Hello.
When we cut 6061 we usually cut HSM 10 percent stepover and then finish by taking .005 of slowly at full depth (provided its not to deep). I now have bunch of parts that I want to cut as fast as possible and yet keep a decent wall finish. Can I do it in one pass? Slot and leave kind of thing. The details are an open ended slot the doc is .25 and the endmill is 3fl .375. What would be a decent feed and speed for this.

Thank you.

I always do a finish pass

10'000 rpm and 150ipm with a 3 flute would be ok. I would start out with a lower feedrate, and increase until I either hit a feedrate I was happy with or if i was breaking endmills. I'd make sure the coolant was spraying along the slot, and would make sure it's flooding the part before it enters.

precisionmetal · Jul 24, 2017

If you can live with a slight radius at the bottom of the slot, an EM with a corner radius will last *much* longer.

My "go-to" end mill in that size is a 29287 Helical. 3-flute, .375" Dia, .500" LOC, .020" corner radius, Zplus coating, and staggered chip breakers cut into the flutes.

Helical says 2200 SFPM, and .0028" feed/tooth in wrought aluminum. That would be 22,000rpm and 185 in/min feed rate. - Yowza!!! - As stated by others, the biggest issue will be clearing the chips.

PM

007Rob · Jul 25, 2017

Milland said:
Hmm - I was an early adopter of three flute EM's back in the old days when C2 was the carbide of choice. Not sure why you don't like it, but to each their own.

I'm a little surprised nobody's come out with a four flute optimized for Al, I bet it could be done with the right helix angle and aggressive geometry to make it sing...

I agree, good 3-flute EM's work great and if you're trying to rough and finish in one operation it just makes sense.

RE: 4-flute EM's with AL geometry, I use some CVD coated endmills from a local company that follow this concept for cutting copper sink EDM electrodes, 4-flute endmill with a nice positive aluminum type grind so you can feed it that much faster than a 3-flute if you don't need the chip clearance. Works great for 3D surfacing at high speeds.

Mtndew · Jul 25, 2017

plutoniumsalmon said:
Hello.
When we cut 6061 we usually cut HSM 10 percent stepover and then finish by taking .005 of slowly at full depth (provided its not to deep). I now have bunch of parts that I want to cut as fast as possible and yet keep a decent wall finish. Can I do it in one pass? Slot and leave kind of thing. The details are an open ended slot the doc is .25 and the endmill is 3fl .375. What would be a decent feed and speed for this.

Thank you.

The TOTAL depth of the slot is .250"?
What machine? What is your max rpm?
Look at most (good) name brand mfg's and you'll find a 3 flute ZrN coated endmill to do the job. Bright Uncoated works too.

OSG
Fullerton
Garr
Destiny (their Diamonback roughers are badass!)
etc...

Milland · Jul 25, 2017

007Rob said:
RE: 4-flute EM's with AL geometry, I use some CVD coated endmills from a local company that follow this concept for cutting copper sink EDM electrodes, 4-flute endmill with a nice positive aluminum type grind so you can feed it that much faster than a 3-flute if you don't need the chip clearance. Works great for 3D surfacing at high speeds.

Well, now you've got me curious - website for this company? I'd like to check them out.

007Rob · Jul 25, 2017

Milland said:
Well, now you've got me curious - website for this company? I'd like to check them out.

Here's the website: Diamond Coated End Mills | Diamond Coated Cutting Tools | CVD Diamond Corporation

My use for these is mostly 3d surfacing using the radius of bullnose tools so I can't speak to their surface finish on deep pockets and that kind of thing but I get pretty decent results for the price, I think.

I do wonder why more companies don't come out with 5+ flute endmills suitable for aluminum, I can't be the only guy who does lots of surfacing in soft materials. Although I guess at some point, you can just program for the max feedrate you can hold and just adjust the rpm to match.

metalmadness · Jul 25, 2017

plutoniumsalmon said:
Hello.
When we cut 6061 we usually cut HSM 10 percent stepover and then finish by taking .005 of slowly at full depth (provided its not to deep). I now have bunch of parts that I want to cut as fast as possible and yet keep a decent wall finish. Can I do it in one pass? Slot and leave kind of thing. The details are an open ended slot the doc is .25 and the endmill is 3fl .375. What would be a decent feed and speed for this.

Thank you.

This topic is pretty well answered buuuuuut 3fl 1/2 coated 37 degree helix at 60ipm...6100 rpm. I think 3 flutes are better but thats just me. Also try a larger finish pass, i usually do a .05 semi finish and a .01 final finish if surface is an important factor.I do this even with 2" DOC

EDIT; as was noted above, separate rough and finish tools will yield better finishes over a longer period.

deadlykitten · Jul 25, 2017

007Rob said:
Here's the website: Diamond Coated End Mills | Diamond Coated Cutting Tools | CVD Diamond Corporation

is interesting, because on that site you can see a boeing, a hunter plane, and a pretty simple part

those just dont go togheter

there is a tool producer arround here, that has a lamborghini and a lame drill on the website

i always specify that i need tools to fix my lambo

007Rob · Jul 25, 2017

deadlykitten said:
there is a tool producer arround here, that has a lamborghini and a lame drill on the website i always specify that i need tools to fix my lambo

Rookie mistake - lambo owner can afford more expensive tools. Better to tell them you need tools to make parts for Lada

plutoniumsalmon · Jul 25, 2017

Mtndew said:
The TOTAL depth of the slot is .250"?
What machine? What is your max rpm?
Look at most (good) name brand mfg's and you'll find a 3 flute ZrN coated endmill to do the job. Bright Uncoated works too.

OSG
Fullerton
Garr
Destiny (their Diamonback roughers are badass!)
etc...

Hello All.

6 K is the fastest I can get. Its a live tooled lathe. The endmill would be from mcmaster (they carry widia I think.Yes the total DOC is.25. With flood coolant.

gkoenig · Jul 25, 2017

plutoniumsalmon said:
6 K is the fastest I can get. Its a live tooled lathe. The endmill would be from mcmaster (they carry widia I think.Yes the total DOC is.25. With flood coolant.

Why McMaster? You can get better end mills for less money from any one of the other 12,729 tool suppliers in the LA basin.

Winterfalke · Jul 25, 2017

007Rob said:
I do wonder why more companies don't come out with 5+ flute endmills suitable for aluminum, I can't be the only guy who does lots of surfacing in soft materials. Although I guess at some point, you can just program for the max feedrate you can hold and just adjust the rpm to match.

Pretty much all I asked for from all of our vendors was a 1/2" 5 flute with an aluminum specific grind. Not one had ever considered it. 90% or more of my toolpaths are under 33% step over because of work holding, I have no need of huge gullets between the flutes. And the rare occasion I did need to hog out material I used an insert tool wherever it would fit. Three flute tools are just not as ridgid or strong, and don't leave as good a finish. I was using the 6 flute EMs for hard alloys as finishers because I could feed 50% faster and get a decent finish in a lot of applications.

gkoenig · Jul 25, 2017

Winterfalke said:
Pretty much all I asked for from all of our vendors was a 1/2" 5 flute with an aluminum specific grind. Not one had ever considered it. 90% or more of my toolpaths are under 33% step over because of work holding, I have no need of huge gullets between the flutes. And the rare occasion I did need to hog out material I used an insert tool wherever it would fit. Three flute tools are just not as ridgid or strong, and don't leave as good a finish. I was using the 6 flute EMs for hard alloys as finishers because I could feed 50% faster and get a decent finish in a lot of applications.

Swift Carb AF5s.

plutoniumsalmon · Jul 25, 2017

gkoenig said:
Why McMaster? You can get better end mills for less money from any one of the other 12,729 tool suppliers in the LA basin.

Hello. Actually I found that their endmills are not terrible, nor that much more expensive. Also it is much faster as a lot of the regular tool suppliers have websites from the early 00's and it takes a long time to call them have them find what you need in their archaic inventory system, see if its in stock, give them a credit card number, wait for their truck to hopefully deliver it today or tomorrow morning and so on an so fourth. With mc master I can order what I need in a minute and be done with it.

One endmill great surface finish in slotting 6061 Question

Hot Rolled

Diamond

Aluminum

Diamond

Titanium

Diamond

Diamond

Stainless

Aluminum

Diamond

Diamond

Aluminum

Hot Rolled

Banned

Aluminum

Hot Rolled

Titanium

Stainless

Titanium

Hot Rolled

Similar threads