[jsanchez177]

I'm trying to drill a .3970 diameter hole .375 deep into 6005 T5 Aluminum using a spindle that lacks power in the lower rpms so I have to feed the cutter into the material at nearly 18,000 rpms. I'm plunging the cutter at 50 ipm which was a feed recommended to me by a representative at Onsrud.

During my first attempts at this I used a single O Flute cutter from Onsrud. They worked great with no re-weld and good chip formation. But the cutter kept breaking about halfway up the shank after about 100 holes. My guess that this break is due to the un-tapered router cutters' flute edge contacting the material throughout the entire plunge, which is putting intolerable stresses on the brittle carbide. With these cutters being nearly 80 bucks a piece, each time one breaks I can't eat dinner that day and I'm getting kinda skinny. So back to the drawing board.

My next idea was to use a tapered Drill cutter and try to slow the rpms down as low as I can. But i'm guessing i'll only be able to get it down to about 15,000 rpms, 10,000 if i'm lucky. This seems to me to be way to fast and that I'll get real short tool life to no tool life at all.

Does anyone have any experience with anything similar to this and have any advice for me?

I appreciate any input. Thank you!

[78nova]

First problem = listening to a tool rep's recommendations. Results = broken tools 99.99 % of the time. These dud's are salesmen, not machinist. Sounds like he has you set up like a punch press instead of actually drilling holes. Honestly, I had never heard of Onsrud tools until I had read your post. Any drill that runs at 18000 rpm @ 50 ipm is going to have some issues eventually. I would recommend a much lower speed and feed along with a peck cycle even with the shallow depth you quoted. You did not specify any hole size tolerance, depth tolerance or hole location tolerances. Fullerton carbide drills are self centering and they work good in 7075 & 2219 aluminum. I am not familiar with 6005.
These drills are very free cutting and would be about $30 cheaper per drill than what you are using now. I would run the fullerton drill at 1500 - 2500 rpm, .150 peck at 6 -10 ipm. These recommendations are on the conservative side since most of the stuff we drill is +.006 / -.001 for the drill hole size tolerances and I like to start out conservative and then see how much I can speed things up and still make good parts. The way you hold the drill and the effective length used are also to be taken into consideration.

I can recall several years ago, a tool rep made a speed and feed recommendation for a Carbide Insert Drill he brought in for us to try drilling a through hole in 15-5 stainless. Even though I had not been in the machining field very long I knew right off we were going to have problems and I told my boss & the tool rep that this was not going to work. The tool rep was so confident in his tool and his suggested speed and feed and my boss said run it. Well that tool burnt itself up before it made it through the part. The look on the tool rep's face was priceless. He went out to his car and brought in another one to try on another part, using the speed & feed I thought would work better. The tool made it through the part this time. Most tools rep's recommendations are based ideal conditions that most of us are not so fortunate to work with.

I hope some of this babble might help.

Kenny

[jsanchez177]

I hear you there about not listening to the sales representatives. I had to speak to several different people before I talked to someone that made any sense. But anyway, you recommended using a speed of 1500-2500 rpm's which i realize is a common speed for a drilling process but i'm unable to achieve a rpm that low with the router spindle that we are using. At a low rpm it doesn't have the torque to drill through a cube of butter.
I may have to end rigging a 8 amp dewalt drill to the spindle plate on our router. haha. Thanks for the food for thought, I enjoy reading the babble of an experienced machinist. Take Care.

[jsheerin]

Are you drilling or pocketing this hole?

That might be something to try - switch to a smaller diameter endmill and pocket the hole. Use a small depth of cut. This has worked for me using my router. You could use a 1/4" endmill for around $10:
http://www.discount-tools.com/endmills/3855.cfm
I think I was feeding around 20ipm at ~10k rpm using a 1/4" 2 flute carbide endmill the last time I was cutting aluminum. That was 6061-T6. I typically set up my cut to spiral down in the middle of the hole for maybe 0.05" of depth and then spiraled out to clean up the OD before going back in to the middle to cut down again. I think I usually go down at a 10degree angle or less. I didn't have many problems with chip rewelding. The only time I'd have problems with that was drilling with an endmill. This would occasionally cause me to break an endmill (when the flutes loaded up with welded material). I could usually fix that by shooting some WD40 in the hole while drilling. It would probably take longer to cut each hole with pocketing, but you'd have to evaluate the trade off in cutter cost versus cutting time.