Small endmill and AL

Corn · Mar 11, 2020

Hi,

I had to mill small slot with 3mm diameter 3 flute carbide endmill and the DOC was 3mm as well. Material Aluminium most likely 6063 T6. No flood coolant in use, just compressed air to blow the chips away. It didn't end up well, I broke the endmill due to chip welding and clogging it. I checked the feeds and speeds by G-wizard and even the lowest setting with limited 7000RPM gave 160 mm/min. I used actually 130mm/min to be safe but didn't help. So my question is, is there any chance to make this work with plain compressed air? Maybe with lower rpm.

Thank you in advance.

Cole2534 · Mar 11, 2020

Instant fix- spray a line of WD-40 in the EM's travel path, direct the air flow to where it will still clear chips but hopefully not remove all the WD-40. Could also be a good place to try one of those machining pastes.

Longterm, upgrade your air blast to include an MQL system.

litlerob1 · Mar 11, 2020

Lowering the RPM won't ever help. I would try a bright shiny Aluminum specific Endmill with 2 flutes, instead of 3. Don't use 1 depth, use as many as needed...

R

tay2daizzo8 · Mar 11, 2020

depth cuts if you want only air

edit:damn Rob beat me to it

Bobw · Mar 11, 2020

gave 160 mm/min. I used actually 130mm/min to be safe but didn't help.

Conventional wisdom failed you. Lower feed to not melt down..

What you needed to do was increase the chip load. That whole getting the
heat out with the chip thing.

A bunch of shallow cuts, and feed the hell out of it.

Also, and I HATE saying this, makes me sound like home shop harry. A little
squirt of WD40, or some other kind of lubricant.. Whatever you have in a can
works, liquid wrench, even a little squirt of tap magic, just something to add
a little lubricity.

Also, you have air, a mist system isn't expensive and it doesn't have to be fancy.

Cole2534 · Mar 11, 2020

Bobw said:
Conventional wisdom failed you. Lower feed to not melt down..

What you needed to do was increase the chip load. That whole getting the
heat out with the chip thing.

A bunch of shallow cuts, and feed the hell out of it.

Also, and I HATE saying this, makes me sound like home shop harry. A little
squirt of WD40, or some other kind of lubricant.. Whatever you have in a can
works, liquid wrench, even a little squirt of tap magic, just something to add
a little lubricity.

Also, you have air, a mist system isn't expensive and it doesn't have to be fancy.

All bundled up for $185. Trico HDPE Lil Mister System with Plastic Line, 1 qt Capacity, 5-1/4" Width x 8-1/2" Height x 4" Depth: Industrial Lubricants: Amazon.com: Industrial & Scientific

Corn · Mar 11, 2020

Ok, shallow cuts would be it. But the story actually continues. After this slot I need run there dia 5mm and 1.5mm high t-slot cutter in that slot. With that tool shallow cuts are not possible. That cutter has 4 teeth. I have had great luck with isopropanol, but then I can't use compressed air to blow out the chips...

huskermcdoogle · Mar 11, 2020

At 7000 RPM with a stubby aluminum specific carbide endmill in full slot you *should* be able to handle 200-300mm/min feed with a two flute, and a depth of 1xd. That said, if it isn't working, back off on the depth of cut to .5xd. You shouldn't have to go much lower than that. Add some sort of lube as mentioned above, a little should go a long way as long as it is consistently getting to the cutting area. Thinner the better.

Also, very often overlooked, but when running small tools it is better to use small system, on-size collets. My preference is to never use anything larger than an ER16 for a 3mm tool and even then it is likely too big. Too many chances for twisting the collet, causing runout and or poor dampening characteristics. I'd go ER11, Slim Hydraulic w/reducer bushing, Shrink Fit, or Big Daishowa Mega Micro Chuck (have had very good success with 3mm tools in ally slotting 12mm deep).

G00 Proto · Mar 11, 2020

6063 is gummy and likes to chip weld... almost as bad as 5052. There is no way around using some sort of oil and probably compressed air. I used to machine mountains of it (small parts held down on a backer board, open machines, no flood). WD40 worked with supervision, but I eventually I just started building a dam around the whole part since it was small, and submerging the part in Tap Magic. A mister worked better than nothing, but I don't feel it had enough lubricity.

ChipSplitter · Mar 12, 2020

As mentioned previously, try a 2-flute endmill with sharp, polished flutes and maybe even a DLC or ZrN coating designed for alu. I have had good success using high pressure thru-spindle coolant. Is there a reason you can't/don't want to use coolant?

WD40 can be a lifesaver, too. It works well for threading on the lathe as well as tricky slotting applications..

Mike1974 · Mar 12, 2020

Harvey Tool - Speeds and Feeds for every tool

This ^ will get you started for speed and feed.
Is 3mm the final depth? If so you want just enough flute length, then choke up ass far as you can.

TeachMePlease · Mar 12, 2020

Mike1974 said:
Is 3mm the final depth? If so you want just enough flute length, then choke up ass far as you can.

Choke the endmill up where?

numberone · Mar 14, 2020

Must be lower rpm to avoid chip welding, and with less cutting depth, maybe faster feed

ricardo_gt · Mar 14, 2020

I machine a lot of aluminum and also happened to me. You need to increase feed, down cut passes and use a mill that handles aluminium, a WNT mill is what you need.

Chris Attebery · Mar 14, 2020

6063 is a PITA. I’d try a single flute cutter with flood coolant, sprayed cutting oil, or a mister with soluble oil mixed in. Increase your feed per tooth and reduce your cutting speed. You want big chips to pull the heat out of the workpiece.

Good luck!

Corn · Mar 23, 2020

Thanks everyone. Took your advice and as I had only ER25 holders, ordered two ER11 holders..

Also AL spesific 3mm one flute and two flute end mills. Looking for supplier in Europe for Trico lil mister as well.. Haven't yet found any. Also getting Aluminum 2007, hopefully it is not that gummy.

Actually got this spesific case done from Delrin as it was ok for this particular job. Saved the cost and effort of anodizing as well. But for the next case hope I'd be better prepared. :popcorn:

litlerob1 · Mar 23, 2020

Chris Attebery said:
6063 is a PITA. I’d try a single flute cutter with flood coolant, sprayed cutting oil, or a mister with soluble oil mixed in. Increase your feed per tooth and reduce your cutting speed. You want big chips to pull the heat out of the workpiece.

Good luck!

Good lord man. If you think 6061 is a pain, you are in the wrong business.

R

Chris Attebery · Mar 23, 2020

litlerob1 said:
Good lord man. If you think 6061 is a pain, you are in the wrong business.

R

Good lord man. Read my post again. LOL!

litlerob1 · Mar 23, 2020

Chris Attebery said:
Good lord man. Read my post again. LOL!

Same difference. 6061 is slightly less gummy than 6063.

R

precisionmetal · Mar 23, 2020

Corn said:
Hi,

..... I broke the endmill due to chip welding and clogging it.

Corn,

You've received plenty of good advice. I'll add that in my experience, the lubrication part of whatever fluid you use is what matters.

I have a Haas MiniMill that I use almost exclusively for prototype work, and I run oil in it, not coolant. I have machined 1100, 6063, 6061, 5052, 7075, and even soft copper -- using end mills from 3-flute .015" diameter up to 16mm, and have never once welded up material on a cutter in probably 5 years of exclusively using oil.

Get some sort of lubricating fluid into that cut, and I believe all your cutter breakage issues vanish.

PM

Small endmill and AL

Aluminum

Diamond

Diamond

Hot Rolled

Diamond

Diamond

Aluminum

Stainless

Hot Rolled

Titanium

Diamond

Diamond

Plastic

Aluminum

Cast Iron

Aluminum

Diamond

Cast Iron

Diamond

Stainless

Similar threads