Breaking small drills in 6061 - what to do?

[SRT Mike]

I figured I'd put this in a seperate thread - I posted a problem I'm having with the surface quality of a 6061 AL octagon shape I am machining. The exterior is an octagon, the interior is a circle. Looking at the top, I am drilling 8 holes - one in each of the triangular "corners" between the inner circle and outside octagon shape. I need to tap them later and I do not have much room to work with. They are for #0 screws, so I was using a 3/64th drill bit (HSS). We're doing 4000rpm (max on the machine) and 1.5ipm plunge rate. We've tried doing it in a full pass and also tried peck drilling. It doesnt help - we tried to drill one piece with 8 holes and snapped 3 bits off in the holes after only 6 holes - not good.

Any suggestions? Machine is a Bridgeport series 1 with retrofit CNC control. No flood coolant. I am using a collet toolholder that fits well.

Do my RPM and plunge speed look correct? I used the suggestions MasterCAM came up with.

Would going to a carbide drill help? HSS drills are .80/ea, carbide are about $3/ea so before I snap a bunch of carbide bits I wanna solve the problem

Would centerdrilling first help? It wouldnt matter if the top of the hole was sligthly oversize because its covered later so I could use a larger centerdrill to start the hole - although the bits didnt seem to be walking at the start of the hole, rather they would break when they were 1/2 way into the hole.

Any other suggestions? Peck drilling is better? What depth should I do in each peck?

Thanks!
Mike

[little bubba]

Your feed sounds good at about .0003-.0004 per rev, speed at about 50 sfm. My guess is that you aren't using coolant and welding or packing chips. If pecking doesn't work, how often are you pecking? Tiny little drills do not take kindly to packed chips, especially HSS. Use the spraymister that you have and peck every .020 to .030. Make sure that you come all the way back to clear and let the air pressure blow out your hole.

As far as carbide vs HSS, anytime I need to use anything small, endmills, boring bars, drills etc, I much prefer carbide, the price difference is rather small on little tools, but the performance is magnitudes better. I really like those circuit board drills if they have enough flute length.

As far as speeds and feeds go, don't let mastercam tell you what to do. Learn how to figure you own surface speed and chipload, it only takes a couple of seconds to figure your feeds and speeds once you establish a Surface Feet per Minute.

[mrainey]

Agree about pecking. You don't say how deep you're drilling, but the deeper you go the more important the pecks become. The flutes on such a small drill will fill up in no time.

I would have guessed the feedrate could go up to more like 3 IPM at 4000 RPM.

[lerman]

Yes, centerdrilling might help.

Any slight error in alignment causes the drill to bend more as it gets deeper. Centerdrilling might help the alignment.

Ken

[HuFlungDung]

Spot drill, short pecks and WD40 or coolant, all good suggestions.

You might also want to think about tapping later. You might want to see if you can use a form tap, as a form tap is quite a bit stronger, does not create chips to cause tap breakage and uses a slightly larger drill size.

[DareBee]

exactly - I think the problem is coolant/lubricant as well. This is critical when drilling aluminum

[Caprirs]

I drill/tap 0-80's in 6061 all the time on my machining centers. If you are willing, try drilling with a #54 drill (.055" dia.) and use a roll/form tap instead of a conventional cut tap. The advantages are no chips from the tapping which is especially important in blind holes and a superior thread because it is cold worked. I drill at 6000rpm, feed at 10ipm, and peck .025". This is with flood coolant. Centerdrilling is critical to keep the drill centered on location and prevents walking. Normally, I use a 1/8" 90 degree spotting drill and go .035" deep to leave a decent chamfer at the top of the hole. Then, drill with the #54 drill at the values above, then the machine rigid taps at 1000rpm to .025" short of the drilled depth.

[The White Fox]

I've read the replies so far, and I it's all good stuff.

(1) I would try using a 1/16 end mill (for this drill size) to make a flat surface.
(2) Center drill / spot but make sure the spot is SMALLER THAN the O.D. of your drill but bigger than the drill web. The drill may walk as the outer cutting edges hit the part first before the drill centers itself causeing great stress when you haven't even engaged the part yet.

maximum pecking (per machinist hand book) is 3 times the drill diameter. For deep holes (relative to drill size) start with heavy pecking, and back off as you get deeper so by the time you are about 3 - 5 times the drill diameter in depth, you should be pecking about 1/2 - 1/3 the drill diameter.

(3) I think you are being too "wimpy" with your feed rate. I feel that you are heating up the metal and the fine chips being created are welding and / or clogging the flutes and won't come out when you need them to. With a squirt bottle of tapping fluid ("Tap Free") or some other free flowing lube, apply liberally like you want to get rid of the lube, try a feed of about 5 or 6 ipm (or a chip load of about .0010 - .0015 inch / rev). If your machine has 4,000 rpm as max, I'd try maybe Fd 3.0 S2500. Also, for this situation, I'd stay with HSS drills as it has a little bit more flex that carbide doesn't have.

I hope this helps - keep us appraised of you situation before you close this Thread

[cfield60]

use alcohol to lubricate the drill. alcohol breaks the seizure that occurs when drilling aluminum.