[mathewepperson]

im working on a haas tm 3 and am drilling through aluminum that is 6 1/4" thick. i was drilling through 4 1/5 " aluminum and the program worked great, but a quarter of the way through the machine stopped because the drill bound up in the hole. probably because of improper chip clearance. then i edited the program and slowed the feed rate down and set the retract height to .2 inch above part. then drilled the same hole and the drill shattered. im using deep hole peck drill taking .075 each peck feed rate was 3.25 then slowed down to 2 after the slip, then the drill broke. is there a better way to clear the chips out of the hole or what am i doing wrong? any suggestions are helpful

thanks,

matt

[Machineit]

You did not mention the size of the drill nor the rpm of the drill and that we will pretty much need.

Slowing your feed is probably what hurt you. Too much time in the hole without coolant and it will bind up.

Make sure that you use full rapid speed and use shorter peck strokes. Short pecks at slow feed make long stringy chips that will clog. A good solid chip will travel up the drill and get thrown off of the drill during the retraction. The longer that the drill is engaged the greater the chance it will max out the power of the machine too.

Give us more details.

Mike

[mathewepperson]

im running 525 rpm. anything above that just makes a bad sound and i dont really like it. and the drill is 17/32

[aadrew10]

How long are the flutes on the drill bit?

- Andrew

[mathewepperson]

What is the diameter of the drill bit and what speed is the spindle turning? How long are the flutes on the drill bit?

- Andrew

im running 525 rpm. anything above that just makes a bad sound and i dont really like it. and the drill is 17/32

and flutes are 6 1/5.

[Machineit]

I don't know if you are doing production or just drilling a few holes. Do you have coolant on it. Sorry, I'm not used to TM mills, always had VF's.

But, if you are just drilling a few holes, program it with a G83 with shorter pecks and higher feeds to help clear chips. Your drill should not slip. Was that in the holder?

Say, G83 Z-????? R.1 Q.03 F10. Up your RPM a little if you can. Don't know your machine. You might consider drilling a pilot hole of about 3/8" to save power on the 17/32nds drill.

Again, don't go slow or you will seize up the drill or load it up with chips.

Good luck learning.

Mike

[mathewepperson]

I don't know if you are doing production or just drilling a few holes. Do you have coolant on it. Sorry, I'm not used to TM mills, always had VF's.

But, if you are just drilling a few holes, program it with a G83 with shorter pecks and higher feeds to help clear chips. Your drill should not slip. Was that in the holder?

Say, G83 Z-????? R.1 Q.03 F10. Up your RPM a little if you can. Don't know your machine. You might consider drilling a pilot hole of about 3/8" to save power on the 17/32nds drill.

Again, don't go slow or you will seize up the drill or load it up with chips.

Good luck learning.

Mike

was running coolant in a drill chucks, but i turned down the end of the drill to .5 and going to try using it in a 1/2" end mill holder. seems like it doesnt have as much wobble doing it that way too.
not really production just running 4 parts with 4 holes each in them along with other things to it. but ill try using small pecks with higher feeds. going to be a little slower but as long as it gets done then ill be happy

[mathewepperson]

ill also try step drilling with a .25 drill since i already have to do it with 2 holes. i know drills are designed for upward chip evacuation but u think that will allow them to fall through the bottom aswell?

[aadrew10]

If I were you, I would have the drill bit in a collet tool holder. I try to avoid using drill chucks for anything larger than 1/2". I'm skeptical about turning a drill bit down to fit properly in a tool holder... Make sure your drill bit is sharp.

To answer your question, I don't think chips will fall through the bottom as well after a .25 step drill.

[mathewepperson]

If I were you, I would have the drill bit in a collet tool holder. I try to avoid using drill chucks for anything larger than 1/2". I'm skeptical about turning a drill bit down to fit properly in a tool holder... Make sure your drill bit is sharp.

To answer your question, I don't think chips will fall through the bottom as well after a .25 step drill.

i really had no choice but to turn the bit down because we only have smaller collets for the one collet holder. my boss doesnt believe in proper tooling for the machine. he is a old school manual guy and dont know much bout cnc. well me neither, but im learning haha only been doing it for 8 months with no proper training but i do appreciate your help. maybe step drilling wont work that gread with the chips

[DaOne]

I think most of it is due to the slow feed. If it was me I would give 1060 RPM with a 9.41 feed a try. If time isnt a factor make your peck depth .05. Make sure your hitting the center of the flutes at a downward angle with coolant to flush off the chips and do a full retract on every peck. Make sure you using a good quality sharp bit. I would really recommend getting a collet holder. Without that bit running true you have no chance at drilling accurate deep holes. Also you should be using a spot drill to start the hole. Without doing that the drill can walk on start. Your drill is held rigid at an offset to the hole and the deeper you get the more side load you get until it finally fails.

[ToyMaker94566]

If I understand all your parameters correctly:

17/32 drill (.5313); 6061 Alum; hole depth 4 1/5? or 4.200(strange to see a 1/5 call-out, it's like saying a 3/16-32 tap instead of a 10-32, it's just not done. ;-). Make sure your coolant is properly mixed, to watery and you'll seize for sure. Running in a drill chuck, (Not impossible nor recommended), here is what I would be starting with:

First, with a hole that deep, definitely spot drill your hole. Then I would drill in about 1/2 to an 1" in with a stub length drill then the rest with your tapper length drill. My feeds and speeds for the the tapper length drill would be

Speed: 2500 rpm

G83 Z-4.2 Q.1 R0 F25.

By keeping your "R" plane low, no chips can fall back in.

Full rapid, don't dittle around in the hole, get in - get out!

The drill chuck is going to chatter with a long drill, a collet is recommended but turning the shank will work fine if you trust spinning it down true.

I don't know much about the TM machines in terms of power but the less you have, the more you'll need to stay up in the RPMs. Takes more torque to spin it slow and a lighter machine will stall under a load. As mentioned above, short quick pecks will get you thru it.

[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