Tips for machining ½" thick 6061 aluminum sheet

I’m curious if the experts around here have any tips for machining ½" thick 6061 aluminum sheet. I’m making a custom vacuum table that measures 24 x 18". I need to make about a thousand 5mm holes in the material (each ½" deep), and also machine some channels for air handling.

I’m planning on using a Speed Tiger ⅛" diameter, ½" cutting height, O-flute tool made for aluminum. I see the immediate problem in that the end mill cutting height is the same as the work piece thickness. I couldn’t find a ⅛" or ¼" end mill (or wider shank) that had a longer cutting height on Amazon!

Any other tips or tricks for machining this on the HDM?


Personally, I would surface both sides of the sheet which would get you well within the height limit of your endmill. I’ve never found aluminum particularly flat or consistent enough in thickness to avoid surfacing it.

The recipes I use for aluminum on my Pro take about 2 minutes per hole in a half inch of aluminum. That’s a long time but I’ve found hole boring to not be entirely forgiving. If you haven’t done so, I would recommend watching this video: YOUR FEEDRATE IS WRONG! – Haas Automation Tip of the Day - YouTube which explains why you need to slow down holes.

Finally, make sure you have good work holding planned.


Buy a 5mm carbide stub drill with a 5mm collet and peck drill them with full retract .050"- .060" peck depth 30 ipm 10k rpm. Add air blast and some lubricant.


Thank you Chris

My holes have been egg-shaped. This will help me choose the right feed for the holes.

1 Like

This is good advice. I think this will create cleaner holes. I picked up a few bits from McMaster-Carr with a coating.

I assume the peck drilling w/ retraction is to help with chip evacuation?

Chris, this was helpful. Thanks for the link.

I’m planning on drilling the 6mm holes first, then screwing the whole block directly to the CNC table.

Something I’ve seen, albeit with an MDF vacuum table, was the 6mm holed were drilled about half way then much smaller holes (say about 1mm or even smaller) from the center of each hole all the way through. That limits the amount of vacuum lost if some holes remain open, but sill give very good holding power. It isn’t the flow of the air, but the vacuum itself that provides the holding power. It doesn’t eliminate the need to cover large areas of vacuum table that is uncovered, but does mean you don’t have to be very finicky about covering ALL holes.

Of course, you would have to clean out all the holes so they don’t become plugged over time with chips, but you’d have to do that, anyway.


Do you have a link to any good quality 5mm end-mills that you can recommend and that you actually tested? I’m getting great results with up to 4mm drills but anything above that just snaps immediately after touching the aluminum.

1 Like

I run these with no issue peck drilling so far 6mm is the largest I have run. You need to run stub drills and watch it to see if it’s trying to walk. If so run a spot drill .010" deep first to keep it centered.

I do shallow pecks with full retracts pulling out .010" above the hole top to clear the chips and allow my MQL to mist the tip each time.

I also should mention have the 2.2kw spindle on my machine but do remote programming on a 1.5kw 24r drilling with a .201" drill with the same settings and it’s done a few thousand holes with no issue.

.043" is the smallest I run also with no issue just 24k and shallower pecks.


I like the idea of doing a shallow spot drill first. What is an MQL?

It’s an air blast setup that sprays tiny amounts of cutting fluid to cool the tool and improve the finish.

.159" and .043" drills I’m running at the moment

I run the bigger drill at 30 ipm not 10 sorry


Good stuff. I’ll give that a try. took me two whole days to bore out 960 m6 holes with 1/8 endmill, because all of my 5mm drills were snapping. Let’s hope this is gonna yield better results.

1 Like

I would suggest using mic-6 or Alca-5 tooling plate as then the overall flatness is done. Then I used a regular drill bit to drill all the holes. Not a big deal for these machines.

1 Like

Thanks - this is helpful!

10K RPM w/ shallow pecks - totally the sweet spot. The 5 and 6 mm stub drills were an awesome investment. Thanks, Able - & Chris


@Able tested 5mm stub drill with your s&f and the results were very satisfactory. Appreciate you sharing the info!

1 Like

@Able right on the money with the 5mm stub. The 6mm kept forcing the spindle to stop. I ended up doing 0.25mm pecks at 10K RPM and 30 IPM and that worked really well.

1 Like

I’m glad you are getting good results. I am curious what the drilling limit difference is between the 1.5kw and 2.2kw spindles are. I ran a 5/16 drill in my 2.2kw just to test at 8k 24 ipm and with a .159" pre drilled pilot hole it worked but the hole finish wasn’t great and with no pilot it only worked for 1 hole before it started loosing steps and I stopped because I don’t want to hurt anything.

I know if I upped the cutting fluid and reduced the peck depth and feed some I could get it to work but it’s not worth it so .25" is the biggest drill I will run on my machine.

I bought the 110V spindle w/ my HDM. At the rates I used above, my finish was quite smooth. I was very happy with the final outcome.

FWIW, in Fusion 360, I also let the spindle run for 1 second at the bottom. That’s supposed to help generate a smoother finish.


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.