What's new
What's new
By:
Advanced search…

How to drill deep small holes in AL6061

ProjectZero

ProjectZero

Aluminum
Joined
Oct 21, 2016
Hi guys,

Looking for some advice on drilling some very small channels in a block of AL6061. Channels are 1" long. I went out and bought the longest 1/32" drill bits the local tooling shop had - 2" long with a .75" cutting length. Yes I'm hoping I can fudge that last quarter inch. Yes this will probably end in disaster.

That aside, I've got it drilling Full Retract with a plunge speed of 7 in/min and a pecking depth of .03125. 10k RPM. I read that the rule of thumb for peck depth was 1x diameter. I'm not dwelling. Nervous about drilling holes so small this deep - anything I can do to improve my chances of success?

Thanks!
 
ProjectZero said:
Hi guys,

Looking for some advice on drilling some very small channels in a block of AL6061. Channels are 1" long. I went out and bought the longest 1/32" drill bits the local tooling shop had - 2" long with a .75" cutting length. Yes I'm hoping I can fudge that last quarter inch. Yes this will probably end in disaster.

That aside, I've got it drilling Full Retract with a plunge speed of 7 in/min and a pecking depth of .03125. 10k RPM. I read that the rule of thumb for peck depth was 1x diameter. I'm not dwelling. Nervous about drilling holes so small this deep - anything I can do to improve my chances of success?

Thanks!
Click to expand...

i would slow rpm, its just creates heat and vibration
 
Drill it at deep as you can with a regular jobber Ø1/32 and use that pilot for your long Ø1/32". If you're going beyond the flutes I wouldn't go more than 1/2D per peck and I'd want to keep the tip of that drill inside the hole, probably want to start the drill inside the hole as well it will be pretty whippy. Long hand it if you have to.
 
Think positive, you can drill hundreds of holes to small $2 scrap alu piece to experiment and fine-tune the values. Something that is not so practical if you have 4" insert drill and 1000 lbs chunk of Inconel. :D

IF you encounter problems take a critical look at the drill. Some of the miniature drills are IMO too coarse surface finish for the size.

This makes it look so easy:
MIKRON TOOL - CrazyDrill Flex - 213_Flexibility_Deep hole drilling - YouTube
 
We have a part with a .032 hole, a little over 1" deep. I use a taper length drill, spot to .046 dia, 9000 rpm, 2ipm, .015 peck.

We've run thousands of them, never broken a drill yet. (change drills about every 100 holes)
 
Larry Dickman said:
We have a part with a .032 hole, a little over 1" deep. I use a taper length drill, spot to .046 dia, 9000 rpm, 2ipm, .015 peck.

We've run thousands of them, never broken a drill yet. (change drills about every 100 holes)
Click to expand...

Awesome. Is the material ALuminum? Do you only peck or do you Full Retract? Do you dwell at the bottom?
 
+1 with hazzert for keeping the drill in the hole. I've had long drills breaks going back in the hole before. It has enough whip to catch the edge sometimes.

That being said, slow rpm, slow feed into the hole, then your cutting rpm, and repeat the process coming out at the end.

And do a good job piloting with the 1st drill. Use a nice stubby one, spot with an 1/8 spotdrill.

I think you can get it 😊
 
Thanks everyone! I spot drilled with a small #1 center drill poking holes about .040 deep. Then I went in with the 2" taper length drill bit and Full Retract pecked by .015. Used a 3 in/min feed rate with .015 peck and no dwelling. So far so good though I won't know for sure until I drill holes on another face and make sure they align. But I'm optimistic!
 
ProjectZero said:
Hi guys,

Looking for some advice on drilling some very small channels in a block of AL6061. Channels are 1" long. I went out and bought the longest 1/32" drill bits the local tooling shop had - 2" long with a .75" cutting length. Yes I'm hoping I can fudge that last quarter inch. Yes this will probably end in disaster.

That aside, I've got it drilling Full Retract with a plunge speed of 7 in/min and a pecking depth of .03125. 10k RPM. I read that the rule of thumb for peck depth was 1x diameter. I'm not dwelling. Nervous about drilling holes so small this deep - anything I can do to improve my chances of success?

Thanks!
Click to expand...


Coolant thru is extremely helpful with any drilling application, especially small and deep holes. Mikron is great, and there are a lot of others with great drills. carbide with DLC or Zrn coating, or uncoated/polished drills are best for aluminum, but PVD works. retracting is bad as the drill may whip and break if it comes out of the hole. running too slow causes chip packing and the drill will break in the hole, but if you dont have coolant thru the spindle, not retracting is going to cause a lot of heat and built up edge and of course breaking. with most drilling applications, the best results are from drilling right to depth. And as mentioned previously, use a standard drill to drill as deep as possible and then put the "Long" drill into the hole at a low RPM (250RPM) and once captured in the hole, speed it up to the proper running parameters.
Never dwell in the hole, and as mentioned earlier pecking is bad....but without coolant thru spindle you can only get away with maybe 3-5 X the diameter successfully not pecking, and going straight to depth.
Another problem with pecking is coming back into the hole and hitting a chip. to prevent that you can peck a percentage of the drill.

depending if your machine accepts macros you can write one to peck at feed rate and back up a given amount to let coolant in, and feed back down.
Or write an incremental sub program and loop it to do the above.

It is doubtful they will align....maybe drill smaller diameter and finish with .031 to pick up drilled hole from other side.

drilled some .008 20X diameter and smaller holes in various materials.....it is a pain in the arse.
 
john-san said:
Coolant thru is extremely helpful with any drilling application, especially small and deep holes. Mikron is great, and there are a lot of others with great drills. carbide with DLC or Zrn coating, or uncoated/polished drills are best for aluminum, but PVD works. retracting is bad as the drill may whip and break if it comes out of the hole. running too slow causes chip packing and the drill will break in the hole, but if you dont have coolant thru the spindle, not retracting is going to cause a lot of heat and built up edge and of course breaking. with most drilling applications, the best results are from drilling right to depth. And as mentioned previously, use a standard drill to drill as deep as possible and then put the "Long" drill into the hole at a low RPM (250RPM) and once captured in the hole, speed it up to the proper running parameters.
Never dwell in the hole, and as mentioned earlier pecking is bad....but without coolant thru spindle you can only get away with maybe 3-5 X the diameter successfully not pecking, and going straight to depth.
Another problem with pecking is coming back into the hole and hitting a chip. to prevent that you can peck a percentage of the drill.

depending if your machine accepts macros you can write one to peck at feed rate and back up a given amount to let coolant in, and feed back down.
Or write an incremental sub program and loop it to do the above.

It is doubtful they will align....maybe drill smaller diameter and finish with .031 to pick up drilled hole from other side.

drilled some .008 20X diameter and smaller holes in various materials.....it is a pain in the arse.
Click to expand...


Hey man thanks for all the info. .008...i don't know how you did that. I ended up pecking by half the diameter, .015, and fully retracting after each peck. I don't have coolant thru spindle unfortunately. Even this isn't perfect, I got through my first part but then broke the drill bit on the part flip. I think it's because I had only made a slight indent with my center drill cause I didn't have the right size. Got a proper #0 center drill and made a 30 thou indent and the next part went all right. I've got my spindle at 9500 and my feed at 2. No dwell. It still is a bit of a gamble. I'm going to try another part and hope it goes ok.
 
Multiple drills, look at a Big Kaiser micro/baby chuck to be down in the channels if possible. Also, if you can get it, while carbide is great, Cobalt will have WAY better performance than HSS. With smaller drills like this, watch the grind on the tip. We've seen drills this size that were "sharpened" with a positive relief. Bust out a course stone and your Opti-Visor and make sure they are sharpened correctly, or buy good drills!
 
ProjectZero said:
But I'm optimistic!
Click to expand...

I have drilled quite many holes to aluminium with dremel style tool..1mm drill and 30xD handheld :D (dremel style gutless tool seems actually pretty good as you get clear indication on pitch/tone depending on load even with 1mm drill)

OK, tolerances and alignment were totally non-critical, just needed to make the holes to fit themocouple to various pieces for temperature measurement.
 
we drill 6061 and some plastics all the time with bits as small as #71 and go well past the flute length all the time. the 2 biggest things you have to keep in mind is rpm because of heat buildup, and chip clearing. To large a peck when going beyond the flute will over fill the flutes and destroy part and bit
 
You must log in or register to reply here.

Similar threads

3
Deep hole threading? 2x one shot or peck tap?
Replies
7
Views
700
Matt G
M
M
Process instability(Boring, Deep Hole Drilling)
Replies
14
Views
1K
CarbideBob
C
S
Carbide drilling with TSC deep holes
2
Replies
28
Views
2K
Mr.Chipeater
M
X
G83 peck canned cycle, doosan lynx. Can I change the point that it rapids back into the hole to?
Replies
9
Views
1K
Fancuku
F
Trboatworks
How true are drilled holes on a lathe?
2
Replies
27
Views
2K
jim rozen
jim rozen








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top