[Pondo]

Drilling a 17/32 hole @525 RPM gives you a surface speed of about 70 SFM.
I start at 100 SFM at the low end for drilling in aluminum and usually run around 200 SFM.
Gotta keep the chipload above .003/tooth and work up from there to whatever the loadmeter says it can handle.
Peck depth varies, I look at the length of the chips and keep them approximately the same length as the flutes of the drill. Shorter if they don't clear immediately or wrap around the drill at all.
The chips should not go downward at all through a pilot hole, but a pilot hole lets coolant flow through and works well for bigger holes (above 5/8"). I run drills up to 1.250" with no pilot hole in aluminum very often though up to 4" deep in my Minimill.
In aluminum, the drill needs to be sharp and the corners can not be damaged (no flank wear). What happens is that the material mushes away and then binds up farther up on the drill. You will see the aluminum on the OD of the flutes and be able to feel it with a fingernail. You can get around this by sharpening the drill slightly off center so it cuts a little bit oversize. Not as much as you need to do with copper alloys, but just a little. Split points work better in CNC machines too (chisel points are for drill presses, not any machine with a Z axis ballscrew IMHO).
LOTS of coolant and it'll work well.

[ToyMaker94566]

Drilling a 17/32 hole @525 RPM gives you a surface speed of about 70 SFM.
I start at 100 SFM at the low end for drilling in aluminum and usually run around 200 SFM.

Ya know, aluminum is an exception to the rules when it comes to feeds and speeds, you can get away with murder on that stuff. Usually machine rigidity and hp will determine what feeds and speeds I run when milling, drilling or turning it. I typically start @ 800 sfm and work my way up. Often times I will end up around 1200 to 1600 sfm and have even run 2400 sfm but I don't think I have ever spun below 800 unless there was some special circumstance where I needed to keep my speed down for part or tool condition like finishes or coolant saturation. Even Machinery's Hand book starts @400 sfm.... I guess I'm just not use to working with machine tools under 15hp.

[Pondo]

Ya know, aluminum is an exception to the rules when it comes to feeds and speeds, you can get away with murder on that stuff. Usually machine rigidity and hp will determine what feeds and speeds I run when milling, drilling or turning it. I typically start @ 800 sfm and work my way up. Often times I will end up around 1200 to 1600 sfm and have even run 2400 sfm but I don't think I have ever spun below 800 unless there was some special circumstance where I needed to keep my speed down for part or tool condition like finishes or coolant saturation. Even Machinery's Hand book starts @400 sfm.... I guess I'm just not use to working with machine tools under 15hp.

Take a HSS drill a 17/32 hole that is 8XDia @1200 SFM (Approx 9K RPM) and .012/tooth chipload (216 IPM - Dead center of the Machinery's Handbook recommendation) and let me know how it turns out. Regardless of how many HP the machine has.

The guy says he has limited experience and specifys that he is running a TM mill, and your #s set him up for failure.

[aadrew10]

Take a HSS drill a 17/32 hole that is 8XDia @1200 SFM (Approx 9K RPM) and .012/tooth chipload (216 IPM - Dead center of the Machinery's Handbook recommendation) and let me know how it turns out. Regardless of how many HP the machine has.

The guy says he has limited experience and specifys that he is running a TM mill, and your #s set him up for failure.

Just to avoid confusion, Pondo is saying you should NOT do this!

[Machineit]

Yup, unless you are going for high speed production with proven machines, drills, coolant and G-code, just keep it simple.

There is no sense in pushing the limit all of the time. He has already had a seized drill and a shattered one, why set him up for more problems. And, his boss does not know what he is doing and is not knowledgeable and has him working with poor drill bits, ground down.

KISS---Mike

[ToyMaker94566]

Take a HSS drill a 17/32 hole that is 8XDia @1200 SFM (Approx 9K RPM) and .012/tooth chipload (216 IPM - Dead center of the Machinery's Handbook recommendation) and let me know how it turns out. Regardless of how many HP the machine has.

The guy says he has limited experience and specifys that he is running a TM mill, and your #s set him up for failure.

8X...? 4X is the rule of thumb and my version has 500-600 sfm and .007 per rev for a 1/2 drill.

So: 4 X 600 = 2400 / 17/32 (.531) = About 4500 X .007 per rev = Around 31 IPM. Now, I would not suggest this RPM for a tapper length drill but this is a perfectly rational and somewhat conservative feed and speed for a machine tool with at least 15 hp in aluminum. So keep your shirt on guy, I was not taking shots at you... But I'm certainly qualified enough to state my opinion. :cheers:

[Pondo]

But if someone does try it, please take a video - it would be really cool to watch!

I didn't convey my message too well. I just wanted to make sure that Matt didn't try to run it with those #'s for his aplication. :cheers:

[Vern Smith]

I drill a lot of aluminum, as previously stated you can go at it pretty hard but if you are welding or breaking the drill then heat is your problem. There are a lot of ways to reduce heat but putting the rapids on 25% giving the coolant some extra time to cool the bit and the work will do wonders for you. Hit the feed hold at the top of a deep hole cycle ( you are using deep hole cycles I hope ) and look at the bit. If there are chips in the flutes you are in trouble and have to change something. I'm using a TM-2 so the comparison should be valid.

Vern

[extanker59]

I don't cut much aluminum anymore but years ago we were doing a lot of it. Trying to bring our cycle time down etc...
Anyway, we got a bad batch of aluminum that was gummy as heck and we just couldn't go fast in it. Maybe his boss bought the cheapest, lousy stuff he could get and he will never get to reach the recommended speeds and feeds.