Tooling choices for small slot

[michaelthomas]

I need to machine an 1/8 wide x 1/4 deep slot around a block in 6061. I have an Onsrud router.

I tried some 1/8" 3 flute high helix endmills, but broke them quite quickly. I used their recommended SFM and chip loads. 24000RPM, and .0015 IPT, or 108 inches per minute in feed. I was running a helical interpolation with .0625 pitch. The part is about 3 x 4 inches. The endmills broke at seemingly random places, and not during direction changes.

I'm pretty green when it comes to aluminum..... but it appeared to be chip evacuation, or the lack of, that was breaking the bits. I can't run flood coolant, but I did use an air stream and some wd-40.

I have used single o flute bits with good success, but I thought I would try these.

Any suggestions on a better technique or tool?

[Superman]

I assume you are using carbide.
Are your cutters un-coated ? ( they must be sharp as possible )

Chip clogging would be your main problem, to eliminate this try going around in 2 passes, ,but increase feed to 180 IPM

At 24K, RPM your cutter must also run true (say 2 tenths T.I.R. [0.0002"])

WD40 is good, it would stop the Al sticking to the cutter

You can create a coolant mist system
- air gun with a T piece screwed onto the front
- 1/16" plastic tube running to a container of coolant,
- this tube connects to the middle of the T
- air runs past the opening, creates a vacuum, sucking up the coolant into the passing air supply

a small squeeze clamp on the tube to control the coolant flow

[michaelthomas]

Yes.....uncoated carbide.

The first time I broke a cutter, I noticed there was some vibration in the head. When I replaced the cutter, I also used a different toolholder and collet. The second attempt did not have any vibration, but the cutter broke just the same. I did not measure the TIR.....I will do that Monday, though.

Overall, my depth of cut was only .0625......are you saying that I should reduce it to .03125 and double the feed?

[runangolee]

Some lubricant definitely wouldn't be a bad idea, to keep from cold welding the almuminum in the flutes.

Alumicut would be best but WD40 works well too, just tends to smoke a lot. Personally I would do what exactly what Superman said with the exception of changing your feed rate.

[Geof]

Lubrication/coolant is essential on aluminum with a small cutter in a slot.

0.0015" per tooth is ridiculous for a 1/8" cutter (I don't care what the manufacturer recommends).

Also for aluminum two flute is often better because it gives more room for chips.

I would probably try a cut like this at 1/16" deep with a feed of 40 or 50 imp.

[michaelthomas]

I contacted Maritool after my failed attempts, and they suggested 8000 rpm and maybe 25ipm if not using high pressure flood coolant. I guess that's about .001 IPT. They also suggested the 2 flute idea.

I ordered some 2 flute endmills and a Noga Mini-Cool dual head system. I guess I will know some more next week after I get it hooked up.

The Onsrud has a brush hood that lowers when the spindle starts via compressed air. I believe I can T into the brush cylinder lines to have the mister turn on and off with the spindle. That way I won't have to manually tend the mister during tool changes. I usually remove the brush hood when doing aluminum anyway because I feel like I need to see whats happening.

Thanks for the replies.

[runangolee]

8000 rpm is ridiculously slow. What is the flute length on the endmills you have coming?

Tool salesmen often have little to no clue about what really works...

[michaelthomas]

I thought that seemed awful slow, too. I figured I would start there and keep increasing the rpm while maintaining chip load and see how far I can go.

The cutters have a 1/2" flute.

I look forward to the coming days when I can describe myself as having "some" real experience with aluminum......rather than none.

[Delw]

if your NOT using flood coolant and only wd 40 try coated in a 2 flute even a 4 flute.
I know people say dont use coated, but damn they work good and gives a better finish too.
Uncoated inserts will gal up way to fast on alum when not using flood coolant.

I run 1/8 ball endmill in some slots that are .375 deep at 20 IPM and 12k rpm 2cuts
or one cut at 8500rpms and 8 IPM ( 2 different machines)