Aluminum drill options

traversamars · Jun 18, 2014

Ok aluminum guys I need some help. Most of my work is tool steel
and stainless so I am lost and salesmen are not helping good.
I need to drill a .315 hole 2 inches deep in 6061 aluminum.
My issue is it needs a 32 finish anyone know of a drill that can achieve
that or am I stuck doing a secondary op? Was thinking double margin
to help burnish as it drills but I am told it might bind and break in aluminum.
This is on a production run of 800 pcs/day so time is of the essence
we are trying to save every second and every penny.

DMF_TomB · Jun 18, 2014

i would think a reamer would be needed. you can try different ways and record data on whats faster assuming somebody where you work has not already done the same thing.
.
you do not mention type of machine lathe , mill, etc ? most machines have speed limitations. also through spindle and through the tool coolant to push chips out of the hole matters. just have chips rubbing on the side of the hole can affect finish. i have also seen where coolant type or concentration can affect hole finish too.

traversamars · Jun 18, 2014

Running on a brother mill tap machine with 1000psi thru spindle coolant mixed at 15%

Guest · Jun 18, 2014

Consistency is going to be a problem even with a good domestic 6061 if chip wrap blocks coolant flow or a wrap around drags against the already drilled hole wall you will get a scored or smeared finish. Most likely you will probably achieve 90% or less good parts using just a drill. I would just add a reamer to remove .005 a side.

DMF_TomB · Jun 18, 2014

traversamars said:
Running on a brother mill tap machine with 1000psi thru spindle coolant mixed at 15%

.
some drills like parabolic drills are better at deeper holes in softer materials as the flutes are bigger and chips can get out easier and they often can run at higher feed rates usually with no peck. also there are carbide drills that can run at much higher rpm and feed if machine can handle it.
.
you might be better off drilling faster the bulk of the material then reaming, not sure how long your machine takes to change tools. some machines its maybe 2 seconds and others it can take a full minute to change tools.

curtis r · Jun 18, 2014

You might look into drills like this straight flute Guhring. I have a friend using this type in his shop doing what you are trying to do. I would love to try some but don't have TSC.

Straight-Flute & Die Drill Bits | MSCDirect.com

Fulcircleny · Jun 18, 2014

Depending on wall thickness, I would consider drilling and Roller burnishing, faster than a reamer, no chips to evacuate, and fast feed.
regards,
Chris

simpleminded · Jun 18, 2014

You may want to try a 3 flute drill, kennametal tf type drill, I used something sililar back in the 90s and they worked fantastic in 6061, beutiful round holes with mirror finish.

Bill

PixMan · Jun 18, 2014

Another straight flute coolant-thru sold carbide option is a Titex A3487-8. Made especially for aluminum, its an 8xD drill and also leaves a near-mirror finish.

toolsteel · Jun 18, 2014

simpleminded said:
You may want to try a 3 flute drill, kennametal tf type drill, I used something sililar back in the 90s and they worked fantastic in 6061, beutiful round holes with mirror finish.

Bill

I do not machine much tin foil either

......I have had good results with a 3 flute drill from M.A, Ford.

Gobo · Jun 18, 2014

Try a three flute M.A. Ford twister. Pretty amazing

SDI-Gary · Jun 18, 2014

We use Kennametal TX drills in 6061 T6511 all the time. Looks like the standard length of 5xD comes in at 43mm max recommended depth. Probably too short for the job you have. May be possible to get longer length as a special if you have the time.

These drills are very fast and leave a good finish. Be sure to check the run out of the drill in your collet. The closer to zero the better for the finish, I think. Good through spindle coolant is a must to get the most out of these drills.

Your 8mm dia. drill would run at about 8000 rpm and around .012" feed per rev.

--Gary

Tonytn36 · Jun 19, 2014

4-land, 2 flute PCD tipped drill, straight flute, through coolant. Currently do this on R2B, S2C, S2Dn but in Ø18 mm size. First drill has nearly 400,000 parts on it so far, still looks new.

traversamars · Jun 19, 2014

Tonytn36 said:
4-land, 2 flute PCD tipped drill, straight flute, through coolant. Currently do this on R2B, S2C, S2Dn but in Ø18 mm size. First drill has nearly 400,000 parts on it so far, still looks new.

400,000 parts thats impressive! What brand are you using?

PixMan · Jun 19, 2014

When you have the spindle speed to run and the number of parts to justify it, PCD tooling is the way to go. Its cost per part for lower quantities is too high, because the difference is that tool life and you don't get lower cost per hole if you never reach the life of either a solid carbide or PCD tool.

Tonytn36 · Jun 19, 2014

traversamars said:
400,000 parts thats impressive! What brand are you using?

I can't remember off the top of my head. I'll try to remember to look it up tomorrow.

Search

Largest Manufacturing Technology Community on the Web

Search

Aluminum drill options

traversamars

Plastic

DMF_TomB

Diamond

traversamars

Plastic

Guest

Guest

DMF_TomB

Diamond

curtis r

Aluminum

Fulcircleny

Cast Iron

simpleminded

Aluminum

PixMan

Diamond

toolsteel

Titanium

Gobo

Titanium

SDI-Gary

Aluminum

Tonytn36

Diamond

traversamars

Plastic

PixMan

Diamond

Tonytn36

Diamond

Similar threads