Drilling 5/64" Hole with 1/16" Endmill in Aluminum

(Pete) #1

Anyone have any recommendations for this? Material thickness is .190". I need to drill a large assortment of 5/64" holes and would prefer to us the CNC. I tried pocketing and got to my 4th hole and broke the cutter. I was stepping down about .019" at a time. It seemed to be going well and then it broke.

Anyone have any suggestions or recommendations?

(Jonathan Anderson) #2

What material are you using? What feeds and speeds? Are you pocketing, boring, adaptive clearing?

(Mad Hatter) #3

I have not used this bit, but I have had great success with all of the bits I have purchased from Drillman1 on Ebay. I would just use the bit and do peck drilling through the material.

(Pete) #4

pocketing with a 1/16" bit about .019" per pass, feed like 10ipm maybe 15000 rpms

(Pete) #5

Thanks for the link! I just assumed they didnt make an endmill this specific. Ill definitly give these a try and just do peck drilling.

Do you think 2 3 or 4 flute would be best for drilling?

(Mad Hatter) #6

Unfortunately, I do not know. I’d hit up @Griff or @Vince.Fab. I only use 0.0781" drill bits in wood for my cribbage boards. Good luck!

(Tom Holgate) #7

You could try the helical drilling. It just ramps down as it cuts around the circle. It’s available in Fusion 360 or Estlcam. I have had some success with that.

(Vince) #8


Helical bore op would probably be the way to go. Unless you want to have fun and buy a carbide drill bit that fits your collet and peck drill.

0.001 chipload, have fun

(Pete) #9

I could buy the 5/64" endmill and peck drill. Wouldnt that be easier/safer than trying to helical bore the hole with a 1/16" endmill?

(Vince) #10

Endmills dont like drilling, they can but not optimal. A bore op will be ramping down constantly and also side cutting. Peck drilling with the perfect size leave little room for chip evacuation and your tool load spikes everytime it plunges

Smooth is reliable, especially with small carbides

That’s a 10 thou pitch, would run all day everyday with a wd40drip or airblast

(Pete) #11

ok, I might stick with the 2 flute .0625" cutter and run the holes via fusion 360s boring set up. I was ramping to .019" doc and pocketing the hole when I broke the cutter. But what you are saying is the smooth consistent helical bore is easier on the cutter?

(Vince) #12

Problem #1 is that that’s almost twice the doc you should be taking on that small endmill. I mean that’s almost 33% width, pretty heavy when you factor in things like total indicated runnout.

Imo set chipload to 1 thou, start height a little above top, in passes adjust pitch and you can even start smaller then work up, lead to center

(Pete) #13

ok thanks for the insight. I will give this a shot and see how it goes. Tough part with this set up is I have about 200 of these holes to drill per setup and I want to reduce cycle time as much as possible since I will have to run alot of them.

(Vince) #14

$40 for 10 pack of carbide drills


edit those might not be great for aluminum but they state they offer others, send them a message

(Pete) #15

so if you could find a carbide drill like this you would opt to peck drill the holes vs. helical bore with a 1/16" cutter?

(Tom Holgate) #16

Do you have a plan C? Peck Drilling with a properly coated drill and a high pressure air/oil blast. There is no room for the chips and no strength for re-cutting them. Still probably the best option. Helical second. Just my opinion.

(Vince) #17

For an accurate hole the drill would probably be better but I haven’t run a drill yet. The endmill would probably need multiple passes and dialing in.

Airblast on both, doesn’t have to be crazy strong. The routers blow a decent amount on their own

(Pete) #18

My plan c would be to drill them on a drill press with a traditional drill and a fixture. I would prefer to just do a tool change on my CNC and have it cut all the holes for me accurately.

I think Ill look into some drill endmills and give that a shot. If that doesnt work out I will go the helical bore route with the 1/6" cutter.

(Paul Alfaro) #19

Even if you spot drill/mill them for a second op (drill) outside of the machine would be great. At least you’ll have them on center per the program/part.

(Pete) #20

ya that might be my plan C with plan D being the fixture drilling. That way you could drill down only like 1/4 or 1/2 the depth of the part and finish it up on the drill press.