Help with CNC drilling in aluminum

[BigD]

I'm hoping to get some advice from a seasoned machinist regarding drilling in 6061-T6 aluminum. I prefer to machine without coolant and like to begin by spotting with a countersink/center-drill. If I can get suggestions for the feedrates and so forth for four different hole sizes, I can guess the rest.

When drilling a through hole in 1/2" 6061-T6 aluminum plate, without coolant, using a HSS drill bit and:

a finished hole size of 1/8":
1) What countersink/center-drill size is recommend (#1 - #7)?
2) How deep to center-drill?
3) Should a through pilot hole be then drilled, if so what size?
4) Using the final 1/8" drill bit:
a) What is the recommend RPM?
b) What is the recommend feedrate?
c) Should I peck, if so how deep per peck?

a finished hole size of 1/4":
1) What countersink/center-drill size is recommend (#1 - #7)?
2) How deep to center-drill?
3) Should a through pilot hole be then drilled, if so what size?
4) Using the final 1/4" drill bit:
a) What is the recommend RPM?
b) What is the recommend feedrate?
c) Should I peck, if so how deep per peck?

a finished hole size of 3/8":
1) What countersink/center-drill size is recommend (#1 - #7)?
2) How deep to center-drill?
3) Should a through pilot hole be then drilled, if so what size?
4) Using the final 3/8" drill bit:
a) What is the recommend RPM?
b) What is the recommend feedrate?
c) Should I peck, if so how deep per peck?

a finished hole size of 1/2":
1) What countersink/center-drill size is recommend (#1 - #7)?
2) How deep to center-drill?
3) Should a through pilot hole be then drilled, if so what size?
4) Using the final 1/2" drill bit:
a) What is the recommend RPM?
b) What is the recommend feedrate?
c) Should I peck, if so how deep per peck?

Thanks for your help and suggestions!

[Jawbreaker38]

What type of tolerance do you need to hold and how deep are you drilling? When selecting a center drill I generally go with a pilot diameter just under the drill diameter you're spotting. My general rule for speeds in most aluminum with HSS drills is 300 sfm. Assuming you're using a standard jobber length drill I'd feed 1/8" diameter drill at .002 per rev. For a 1/4" drill I'd feed it at .004 per rev. and a 1/2" drill I'd feed at .007 per rev. As for pecking it depends on the depth you're drilling. If it's more than 3 times the drill diameter I'd start pecking at half the drill diameter. This is all pretty general and there are many other variables.

[BigD]

Jawbreaker38,

Thanks for the reply!

My tolerances are not tight. In my examples, I assume a hole depth of 1/2", with a standard jobber length drill.

You recommend a center drill just smaller than the finished hole size. How deep do you go with your center drill?

Did I do the math correct? If so then you are recommending:
1/8" drill at 9200 RPM with a feedrate of 18 IPM
1/4" drill at 4600 RPM with a feedrate of 18 IPM
1/2" drill at 2300 RPM with a feedrate of 16 IPM

Now my spindle will not go 9200 RPM, then would you recommend something like:
1/8" drill at 5000 RPM with a feedrate of 10 IPM

[TOTALLYRC]

I do a lot of non critical 3/8" hole in 60661-t6 aluminum for a customer job. part is about .300 thick.
I use a jobber lenght drill with no spot, but I normally peck between .050 and .075 to keep the chips short and make it easier to clean up.It also keeps them from wrapping on the bit and throwing coolant all over the place.

[Jawbreaker38]

Originally Posted by BigD Jawbreaker38, Thanks for the reply! My tolerances are not tight. In my examples, I assume a hole depth of 1/2", with a standard jobber length drill. You recommend a center drill just smaller than the finished hole size. How deep do you go with your center drill? Did I do the math correct? If so then you are recommending: 1/8" drill at 9200 RPM with a feedrate of 18 IPM 1/4" drill at 4600 RPM with a feedrate of 18 IPM 1/2" drill at 2300 RPM with a feedrate of 16 IPM Now my spindle will not go 9200 RPM, then would you recommend something like: 1/8" drill at 5000 RPM with a feedrate of 10 IPM

Your speeds and feeds look like a good starting point to me.
But let me try to be more clear with spotting. With the center drill you'll want to go with a body size larger than your drill diameter and leave a chamfer bigger than your drill diameter. My philosophy is that the chamfer captures the outer corners of the drill and pulls it straight. Also you'll be de-burring the drilled hole. Off the top of my head I can't tell you how deep to go with specific # center drills. I select a center drill with a pilot diameter just under your drill size. Always try to spot larger than your drill diameter.
Some may have some more detailed and better information, but this seems to work well for me.
Hope this helps.

[BigD]

Thanks again Jawbreaker38. I think I understand your approach to spotting.

Now if you are drilling a 1/2" hole, let's say 1" deep, would you not drill a pilot through hole? If so, do you have any rules of thumb for the pilot hole?

[Geof]

In aluminum using a drill with a split point you will not need pilot holes for any size up to 1" and maybe even larger; just use a spotting drill to make a starting spot out to about two or three times the size of the web on your drill and then go straight in. Use the speeds, feeds and peck suggestions that have been given.

[BigD]

Thanks Geof!

Then you recommend using a split point bit for drilling in aluminum and skipping the pilot?

Would a good choice for aluminum be something like an uncoated Cobalt Steel 135 degree split point screw-machine drill bit? Or would you prefer a different type?

[Geof]

Uncoated, yes and you really don't need to go to the expense of cobalt on extruded stock such as 6061. The only other thing you might consider are the parabolic flute drills because they are supposed to eject the chip better, we don't use them because we rarely drill really deep holes.

[littlerob]

Originally Posted by Geof Uncoated, yes and you really don't need to go to the expense of cobalt on extruded stock such as 6061. The only other thing you might consider are the parabolic flute drills because they are supposed to eject the chip better, we don't use them because we rarely drill really deep holes.

I think he said he was only drilling 1/2" deep.

If you are drilling only 1/2" and have the access to 135 degree split point screw machine drills, drop the center/spot drill. Hit it hard keep it as cool as you can, you are not going to ruin or work harden 6061. Definitely uncoated and sharp!!

[kling8]

I just read bits and pieces but in alum. here is what I do if possible. no pilot hole no pecking, no HSS I use carbide ram it hard, Hss can walk tool changes and pecking add time. Carbide goes a lot faster, and you should get a lot longer life. Speeds and feeds charts can get you in the ball park and fine tune speeds and feeds from there.

[MDLang]

BigD,

Jawbreaker38 has good feed/speed recomendations. My only recomendation is to definitely use coolant or aluminium cutting fluid. Running dry will almost certainly plug the flutes of the drill running at reasonable rates. If you want to run dry you'll need to slow the speed down quite a bit and watch for plugged flutes.