Melting Aluminum and Clogging Endmills

jbrowne · Feb 12, 2015

We are working with 1/8" to 1/4" aluminum stock on a Bridgeport with an original Prototrak doing basic 2D patterns. We have recently run into some major issues with endmills melting the workpiece and getting clogged with aluminum, stalling the servos/moving the workpiece. This is happening with both two and four flute endmills.....with coolant (emulsified oil) applied at a constant rate from a spray bottle.

The following occurred while using a 1/2" 2 flute endmill at 1115 rpm and 3ipm feedrate. I know this is a low feedrate, but we ended up there after backing off from 8ipm to 5ipm and down to 3ipm, still applying constant coolant from a spray bottle. This was the third "stall and melt" incident on this piece....just normal 6061 extruded stock with 1/8" wall. A 1/2" 2-flute bit should be tearing this thing up, but we kept having awful cutting results??

We have encountered the same problems on brand new US made TiN coated 17/64ths two flute mills to 1/2" uncoated mills....we keep melting the workpiece.

Are we feeding too slow and letting the bit linger in the hot zone on the workpiece? My reaction to these incidents has been to reduce feedrate from theoretical max (using 0.004" per tooth)...but maybe I should be increasing? We were working at 300sfpm and backed off to 250/200. We found a reduction in chatter/squealing, but no improvement in the melting problem.

Thanks for any advice!

g-coder05 · Feb 12, 2015

Assuming you are using a Bridgeport with 4K spindle you should run at 17.28 IPM. If you are having problems with chatter then I would recommend an odd number of flutes 3 or 5. 3 flute should run 24IPM. I do an op like yours quite often in near dry situation an have no problem even in a vice.

358Mustang · Feb 12, 2015

The endmill IS turning the right way right??? LOL

BigHoss · Feb 12, 2015

How sure are you about that being 6061 T6, did you get certs? That behavior mimics some of that crappy hardware store ??? O grade aluminum.

NAST555 · Feb 12, 2015

Look for a dedicated Aluminium endmill if you have not yet.

I do not do a lot of aluminium cutting but when I do it is only with aluminium specific endmills. Super sharp, uncoated and you will see that the helix and clearance to the flutes differs from standard endmills. Another thing to think about is that if at all possible make a small enclosure around the job on the table and blast the crap out of it with as much coolant as your machine can get to it.

Your RPM is also way too slow. I would bump it up to the highest that you are comfortable running the machine at. I run a 10mm (roughly 3/8") at pretty much max RPM,dependent on machines this varies from 4 000-11 000RPM, and just hone the feed in to suit. You know it is close to the sweet spot when you can actually see the coolant blasting nice uniform chips up and away from the endmill.

Marnic · Feb 12, 2015

I also agree that you are running way to slow.
I do a lot of aluminium cutting and the only times i get a problem like this is when there is not enough coolant or like BigHoss says,when its really crap ali.

Ranchero50 · Feb 12, 2015

Speed 1800-2400 Feed 8-18 ipm dependent on the DOC and how well it sounds. I'd also run a 4 flute vs. a 2 flute. You need to make sure the chips are not getting cut twice.

As a new guy I'd also run shallower DOC until you know what the cutter and machine are happy with.

adama · Feb 12, 2015

coolant needs to be decent strength, not piss water too. better yet try wd40, works well

Skarsaune · Feb 12, 2015

You didn't mention, but carbide or HSS end mills? Way too slow, agree that you should be spinning the spindle as fast as you are comfortable with on the machine.

Limy Sami · Feb 12, 2015

Sounds like shitty material BTDT and it's a PITA.
Try switching to kerosene as a cutting lube - not so nice I know but it's got me out of many holes with gummy ally.

P.S. WD40 works just as well - more $$ though.

i_r_machinist · Feb 12, 2015

Get a couple of air misters to blow the chips out while cutting. I'm limited to 5K on my spindles also and the misters work. You have to get the chips out. Dab a little molly dee on uncoated endmills.
have fun
i_r_

TeachMePlease · Feb 12, 2015

Ranchero50 said:
Speed 1800-2400 Feed 8-18 ipm dependent on the DOC and how well it sounds. I'd also run a 4 flute vs. a 2 flute. You need to make sure the chips are not getting cut twice.

Curious about this, as I don't have much experience slotting aluminum, but I was under the impression that fewer flutes = larger gullets = better chip evacuation, which is ideal for ops like this in aluminum. Thoughts?

bukwerm · Feb 12, 2015

I agree with the too slow feed. Cutting slow in a thin wall seems to really concentrate the heat. I regularly do a job that involves cutting windows in the (about .125" thick) walls of 6063 aluminum extrusions. Using aluminum specific emills I run them at 10k rpm and 250ipm. I've ran it both dry and with flood coolant. Slightly better finish with coolant but acceptable dry. When I started running these they were programmed much less aggressively and would gall like your pic if ran dry. I realize you don't have that much rpm, but the point is you can feed like crazy through thin aluminum if you can clamp it well. There's barely any chip to pull the heat off and it's fairly easy to get the chips out of the way. I'm pretty sure my ipm could be increased even more.

The coating could be part of your issue to. I can't say exactly which coatings stick but many that work well in steel will gall up bad in alum. In the above case I use either uncoated or zirconium coated.

Big B · Feb 12, 2015

Are you running a hi helix end mill. If not, you should try that.

Big B

Larry Dickman · Feb 12, 2015

TeachMePlease said:
Curious about this, as I don't have much experience slotting aluminum, but I was under the impression that fewer flutes = larger gullets = better chip evacuation, which is ideal for ops like this in aluminum. Thoughts?

This is true, I would never use a 4 flute on aluminum except maybe on a finish cut. This here, is without question a job for a three fluter . From your photo, it's really hard to believe your having problems, I know it may sound funny, but really, are you sure the cutter's turning the right way? Your cut looks horrible. My next guess would be your material is not what you say. Could it be 6063?

Mtndew · Feb 12, 2015

TeachMePlease said:
Curious about this, as I don't have much experience slotting aluminum, but I was under the impression that fewer flutes = larger gullets = better chip evacuation, which is ideal for ops like this in aluminum. Thoughts?

You win the K car!
The helix angle has a lot to do with it also. A 4 fluter is just asking for trouble unless maybe finishing a wall. I always use 3 flute bright finish carbide and never have an issue unless I try to do something stupid like do a quick cut without coolant just because i'm in a hurry.

SND · Feb 12, 2015

5052 will happily do that for yah, or 6061 with a completely screwed up ht process that turns it to gum.

behindpropellers · Feb 12, 2015

jbrowne said:
We are working with 1/8" to 1/4" aluminum stock on a Bridgeport with an original Prototrak doing basic 2D patterns. We have recently run into some major issues with endmills melting the workpiece and getting clogged with aluminum, stalling the servos/moving the workpiece. This is happening with both two and four flute endmills.....with coolant (emulsified oil) applied at a constant rate from a spray bottle.

The following occurred while using a 1/2" 2 flute endmill at 1115 rpm and 3ipm feedrate. I know this is a low feedrate, but we ended up there after backing off from 8ipm to 5ipm and down to 3ipm, still applying constant coolant from a spray bottle. This was the third "stall and melt" incident on this piece....just normal 6061 extruded stock with 1/8" wall. A 1/2" 2-flute bit should be tearing this thing up, but we kept having awful cutting results??

We have encountered the same problems on brand new US made TiN coated 17/64ths two flute mills to 1/2" uncoated mills....we keep melting the workpiece.

Are we feeding too slow and letting the bit linger in the hot zone on the workpiece? My reaction to these incidents has been to reduce feedrate from theoretical max (using 0.004" per tooth)...but maybe I should be increasing? We were working at 300sfpm and backed off to 250/200. We found a reduction in chatter/squealing, but no improvement in the melting problem.

Thanks for any advice!

Another example of if you have a hammer...everything is a nail. Waterjet. Laser.

NAST555 · Feb 12, 2015

TeachMePlease said:
Curious about this, as I don't have much experience slotting aluminum, but I was under the impression that fewer flutes = larger gullets = better chip evacuation, which is ideal for ops like this in aluminum. Thoughts?

Yup,yup and yup... Most of the sizes,6mm and up, that I use for aluminium are either 2 or 3 flute. And like MtnDew said the helix also comes into play to get the chips up up and awaaaaaay from the cutting area.

I've found the sharper the flutes are and without coating works the best (like I said the aluminium specific endmills). I'm pretty sure that the guys that develop the grinds know A LOT more than me so I trust them and it works

They sure do last a really long time when used properly.

toolsteel · Feb 12, 2015

Larry Dickman said:
This is true, I would never use a 4 flute on aluminum except maybe on a finish cut. This here, is without question a job for a three fluter . From your photo, it's really hard to believe your having problems, I know it may sound funny, but really, are you sure the cutter's turning the right way? Your cut looks horrible. My next guess would be your material is not what you say. Could it be 6063?

3 flute gives a balanced cut.....2 flute works...but wont run as smoothe as a 3 flute will.

Melting Aluminum and Clogging Endmills

Plastic

Titanium

Cast Iron

Aluminum

Stainless

Plastic

Cast Iron

Diamond

Aluminum

Diamond

Titanium

Diamond

Cast Iron

Diamond

Titanium

Diamond

Diamond

Stainless

Stainless

Titanium

Similar threads