[jmc2010]

I have some aluminum extrusions (t-slot table top slats for my cnc) that I need to drill, and counterbore. I want to do this using the cnc. I've purchased a 1/4" drill mill, and a 1/2" drill mill to do the job. Everywhere that I look, it shows the spindle RPM for the drilling and counterboring to be well under my minimum, which is 6000 rpm. This is what I have figured so far, using HSMAdvisor. I have no idea if its even near right, as I've never cut or drilled aluminum on my cnc before.

1/4" drill mill, all the way through .5":

Recommended Peck: 0.12 in (Not Required)
Breakthrough Amount: 0.125 in
Material: 6061-T6 Aluminum 95 HB
Tool: 0.250in 2FL Carbide Jobber twist Drill
Speed: 392.5 SFM/ 6000.0 RPM
Feed: 0.0015 ipt/ 0.0030 ipr/ 18.19 ipm
Reference Chipload: 0.0034 in
Power: 0.3HP
MRR: 0.89 in^3
Torque: 0.23 ft-lb
Max Torque: 1.85 ft-lb

1/2" drill mill, .25" counterbore

Recommended Peck: 0.25 in (Not Required)
Breakthrough Amount: 0.250 in
Material: 6061-T6 Aluminum 95 HB
Tool: 0.500in 2FL Carbide Jobber twist Drill
Speed: 785.0 SFM/ 6000.0 RPM
Feed: 0.0025 ipt/ 0.0050 ipr/ 29.75 ipm
Reference Chipload: 0.0054 in
Power: 1.7HP
MRR: 5.84 in^3
Torque: 1.50 ft-lb
Max Torque: 14.82 ft-lb

Any recommendations would be helpful. I do have a test piece of 6061 to make test cuts on, I just don't want to tear up an mills trying numbers that I guessed at.

Thanks,

Jason

[zero_divide]

For a drill your feed numbers seem quite slow (did my calc give those numbers to you? edit: never mind, i see you are using feed override).
BUT considering this is just an endmill with a pointy tip, i think it will work out ok.

BUT i hope you have coolant and you peck often to prevent chips from clogging.
Because it is not a real drill, you will not have proper chip clearance. Especially for deep holes.

And that 0.5" deep hole seems like it might cause you trouble unless you peck.

This can also be done dry. But for that you will have to go really slow RPM -wise. IMO it is easier to drill steel dry than aluminum.

[jmc2010]

I've already run into some issues with the .5" hole. I was trying to keep within the specs of what the manufacturer wanted for the sfm and feedrate for their drill mills, and that's why I used the feed override. The drill works great until it gets in about .25" of the way, and then it stalls my spindle and my z axis starts losing steps. I also tried upping the rpm to 8000 and the ipm to 25 ipm, but it still stalled. I'm brand new to all of this, so I apologize for my ignorance, but should I be peck drilling this then? I am drilling dry, and everything I've read so far says no need to peck unless my DOC is 3x the diameter of the cutter, so I didn't consider it.

[zero_divide]

I've already run into some issues with the .5" hole. I was trying to keep within the specs of what the manufacturer wanted for the sfm and feedrate for their drill mills, and that's why I used the feed override. The drill works great until it gets in about .25" of the way, and then it stalls my spindle and my z axis starts losing steps. I also tried upping the rpm to 8000 and the ipm to 25 ipm, but it still stalled. I'm brand new to all of this, so I apologize for my ignorance, but should I be peck drilling this then? I am drilling dry, and everything I've read so far says no need to peck unless my DOC is 3x the diameter of the cutter, so I didn't consider it.

Yes. As i said you should be pecking ALOT when drilling dry.
Use some coolant too. Even a spray bottle of WD40 will make things MUCH better.

Also as i said, mill-drills suck big time in both milling and drilling.

If you only need holes, you should have bought cobalt stub drills.
You would not be able to drill through 0.5" dry in one shot anyway.
0.125" pecks at least are required.

Good luck!

[jmc2010]

If you only need holes, you should have bought cobalt stub drills.
You would not be able to drill through 0.5" dry in one shot anyway.
0.125" pecks at least are required.

Good luck!

Ok, I tried just about everything that I could imagine, except using a coolant. I'm not quite setup for that yet, so I want to avoid the mess if at all possible. I tried using a peck every .125" with a .05" chip break. I tried the same peck with full retract. I tried a peck every .0625 with a chip break of .05", and then a full retract on that as well. I tried upping the speeds as well, and nothing really seemed to work. Just about the same depth every time, and the spindle would stall. Very frustrating. I'm glad that I used a scrap piece of aluminum for my test drills. It is now swiss cheese.

Tomorrow, I'll order cobalt stub drills. Is there a coating that I should be getting to make easy work of this aluminum? I'm all in for whatever I need to get the job done right.

Jason

[zero_divide]

TiB coating is exxelent on Aluminum

[jmc2010]

TiB coating is exxelent on Aluminum

I ended up with some hartel screw machine drills in bright. I'll keep the TiB coating in mind for the future. So when calcing the feeds and speeds for these drills that are coming in today, do I just use the jobber drill feeds and speeds in your calc? I only ask because I know these aren't jobbers.

[zero_divide]

Yes its the same.

I always drill at 150% feed override. but giving how weak your spindle is, i bet really small pecks would work best

[jmc2010]

Yes its the same.

I always drill at 150% feed override. but giving how weak your spindle is, i bet really small pecks would work best

The stub drill worked great with the standard speeds and feeds. I am trying to countersink with a 1/2" drill mill now though, and the same thing as the other drill mill. It really seems like either the rpm is too slow, or the feeds are too fast. I'll post up a video later, but its taking huge bites out of the aluminum, and it seems to just push too fast until it just can't cut anymore, and stalls out. The spindle is a 2kw, almost 3hp. It really suprises me that it stalls. With the 1/2" drill mill, I went 9200rpm and 41.60ipm. After it stalled, I reset my z axis 0, and ran it again at 9200 rpm and 22.4ipm, and it didn't stall, but the cut was pretty rough. Should I keep dropping the feed?

Jason

[jmc2010]

This is what it was doing with the 1/2" drill mill:



Ended up getting the 1/2" countersink looking good by going with the following:

Material: 6061-T6 Aluminum 95 HB
Tool: 0.500in 2FL Carbide Solid End Mill
Speed: 1800.0 SFM/ 13758.0 RPM
Feed: 0.0015 ipt/ 0.0030 ipr/ 41.60 ipm
Chip Thickness: 0.0015 in
Reference Chipload: 0.0045 in
Engagement: DOC=0.140 in WOC=0.500 in
Effective Dia: 0.500 in
Cross Section: 0.2800 x Dia.
Power: 1.0HP
MRR: 2.91 in^3
Torque: 0.37 ft-lb

It ends up being 13758 rpm @ 20.8 ipm plunge. Not sure if this is right, but it got the results I'm after. Seems like I may even be able to get the speed up a little more than that even, for a smoother finish.

[jmc2010]

Well, I thought that everything was working great. The test cuts in my 6061 aluminum test piece were working out great. Tonight, I changed to the real work piece that I'll be using and started the spindle up to cut my first holes.. Now even the 1/4" stub drill is stalling my spindle. The work piece is 6063, which is supposed to be a bit softer. I tried the speeds and feeds that worked on the 6061, then I tried slowing the feed down some, then I tried going all the way down to most drill bit manufacturers starting point feeds and speeds for aluminum, and still nada.. This is driving me nuts.. Seems like the chips got WAY bigger.. Here is a pic after I pulled the bit out, and an ER20 collet for size reference.



Attachment 242730

[zero_divide]

Man, this is no chip. This is molten aluminum.
Your spindle is far too weak at slow RPM and when you ramp jp the RPM, you still can not feed fast enough and spindle stalls.

You try to reduce feedrate and instead melting aluminum.

Try coolant.

For 1/4" cobalt drills i would sometimes on a REAL machine go 7000 rpm, 120 ipm. but that is with flood coolant.

there is no way you are going to get thru as such high RPM.

If you reduce the RPM, you might be able to feed light enough to keep your spindle from stalling and keep your material from melting

edit: try 5000 RPM and 6.0ipt
Take 25 thou full retract pecks. Brush the drill with ,some cutting oil before every hole

[jmc2010]

So that is from the feed rate being too slow? I was at 4586 rpm and 41.27 in/min I believe, when I made that cut. I tried halfing that feed and the molten lava pieces were twice as long.. Do I just need more feed speed?

[popspipes]

I drill hundreds of holes in 6061 using flood coolant

.112 drill 3500 rpm 3 ipm with peck at .060 full retract .5 deep, all are through holes.
.170 drill at 1500 rpm 4 ipm .5 deep
.196 drill at 1500 rpm 4 ipm .5 deep

6061 doesnt drill well without coolant, if the rpm is too high it will stick to the tool as it heats up.