countersinking and chamfering aluminum

[michael.sershen]

I've been having some trouble getting clean countersinks and chamfers in aluminum. The result is a bad finish, the AL (6061) looks smeared across the surface and also pushed up over the top edge of the feature.

Here is the tool I've been using:
Mcmaster: 2944A572
carbide, six flute, 3/4" od, 82 deg, TiCN coated
it was $84!!

First, I was trying to countersink a thru hole for a 4-40 hole. I don't remember the speed or feed, but it was based on Gwizard. Aluminum was smooshed out of the hole and left in the flutes of the bit.


Second I tried chamfering the inner edge of the 4"diameter hole. 4000 rpm, 40 ipm, .025 chamfer. The bit was cutting using its .375 diameter. The result was better, but still rough.
I was not sure how it put this into G-wizard, there is no chamfer bit, so i just used "carbide EM". It wanted max rpm and max feed... I chickened out and set it lower.


Is this a speed/feed issue? Am I using an incorrect bit? Is the bit toast? (maybe from abuse on our old smithy)

I have attempted to add a picture of the bit:

Thanks for your suggestions.

[pete from TN]

I have never had much luck with multi flute champfer bits. Especially on the smaller diameter near the point just not enough chip clearance on the flutes to clean adequately. You might try a single or two flute champfer mill. There are lots of them for reasonable prices. If you are smearing metal that is a guaranteed sign that you are not clearing chips and melting metal to the cutters edges welding it in place. Are you using coolant as well? I have seen some good success in youtube videos with two flute triangular insert champfer mills at full stink spindle speed and a slightly slower feedrate. Have not tried it myself but intend to soon. Good luck and peace

Pete

[Gerry Sweetland]

+ 1 on what Pete said.
I have had pretty good luck using the 2 flute solid carbide 90° end drill mills for spotting and chamfering from Enco.
Enco - Guaranteed Lowest Prices on Machinery, Measuring Tools, Cutting Tools and Shop Supplies

I use "Carbide Spot Drill" for the tool in G-Wizzard to get an idea on feed and speed, usually high RPM but slow down the feed a bit. These end mills do very nice chamfering.

I use a HSS 82° 1 flute countersink tool that I got from the local mill supply for like $3 for a .25" Ø tool. These work well for countersinking up to .25" holes.

I also have a .375" and .5" countersinks like that, IIRC they were only a couple of dollars more but I have not had a chance to use them yet.

Gerry

[MetalShavings]

I've had the same problems with countersinking some 6/32" holes on aluminum as well.

After some trial and error experimenting I ended up using the RPMs that were calculated for the diameter of the mouth of my counter-sunk holes; and very shallow peck drilling operations. I'm using a three flute HSS 90 degree counter sink.

My counter sink holes still show signs of what I can only describe as light chatter marks but, nothing as bad as my initial attempts. And, any marks that do exist are covered over with my screw head.

On my initial attempts at countersinking these same size holes it almost looked liked I had broached my counter sinks.

The machining marks were such that the mouth of my counter-sunk-holes looked like the outside edges of pop-bottle caps. (Serrated)

They're much better now.

MetalShavings

[philbur]

Greatly reduced rpm works for me.

Phil

I've had the same problems with countersinking some 3/32" holes on aluminum as well.

[Gundawg]

I like to countersink using an aircraft micro stop countersink tool after the holes are drill by the CNC. That won't help on the 4" hole but they work great for the small holes. They are expensive new but I have found them on ebay for cheap.

Mike

[TXFred]

Regarding Michael's problem, I think his spindle speed is too fast.

Six flute countersinks are great for hand use. They don't chatter. But for CNC, I'll run a two or one flute tool.

My 90 degree tool is a 3/8" Accupro, two flute carbide. To get spindle speed, I figure out the diameter of the tool where it will be cutting, by the formula

Chamfer width + (2 * Overhang) = Cutting Diameter

That tells me the diameter of the chamfer mill at the centerline of my chamfer cut. Then I work out the correct spindle speed for an end mill of that diameter.

Feedrate depends on the quality of the chamfer I'm after. I try not to exceed 0.004" chip load for rough work, such as a fixture. Finished products get a chip load of 0.001" - 0.002" so that they'll look good.

Frederic

[Toad]

I use a 6 flute 1/2" dia. carbide c'sink from Lakeshore Carbide on 6061 aluminum. I had the same problem until I drastically slowed the speed and feed down. I run it at about 600 rpm and very low feed rate around 6 IPM. Also hold the countersink in a collet for min. runout. If you call Lakeshore they are very helpful in solving problems.

[Don Clement]

I have had excellent results in countersinking 6061-T6 on my Tormach using an M A Ford series 60 single flute countersink and Relton A9 fluid. M.A. Ford Carbide Countersinks A-9 Metal-Cutting Fluid

Don