.026 Dia. holes in Aluminum

bmink72 · Dec 19, 2007

Has anyone tried to drill and ream thousands of .026 dia. holes thru 1/4" thick 6061 Al. If so, how much trouble is it going to be and what kind of running parameters and pecks would I need? Also what would be the best tooling?

gdgambler · Dec 20, 2007

reaming alum

I drill and ream thousands and thousands of holes in 6061 t6. I don't know if this will help but my hole is larger in dia. .1675. I drill first with a carbide drill and leave about .003 to .005 on each side to ream. I move the reamer in and out fast. I ream .650 deep with a floating reamer holder with no pecks. The hole appears to be very smooth thru my inspection microscope. Good luck

bmink72 · Dec 20, 2007

My main concern is with the hole being .026 dia. I'm not sure if chips are going to be a big problem. And even though the hole is only .25 deep, that's still almost 10x dia.

g-coder05 · Dec 20, 2007

You could use a kennemetal drill/ream and eliminate 1 op. if you have tsc use an er coolant collet and dont peck. its also gonna depend on your spindle max rmp. a drill/ream that small is gonna need to run WAO.

TRRINO · Dec 20, 2007

Not sure what max spindle is on your machine but you will need lots of RPM.We drill 6AL4V titanium .0225 dia X 1.250 deep. thousands a day. 22,000 rpms with a MA. Ford carbide circuit board drill. Hold +.001 -.0002. Why ream unless for finish. Your trouble will be at break thru--Slow down there or come back with a solid carbide reamer or flat bit chucked up short as possible.

bmink72 · Dec 20, 2007

What kind of feed are you running with the circuit board drills. Do you slow you're feed on entry. I don't need to ream as long as I can hold +/-.001.

Madlab · Dec 20, 2007

TRRINO said:
We drill 6AL4V titanium .0225 dia X 1.250 deep. thousands a day. 22,000 rpms with a MA. Ford carbide circuit board drill. Hold +.001 -.0002.

I have a new Hero...... and he lives in Pa. I have heard M.A. Ford made good drills ... now I have to try some out. 1.25 deep wow........ good work TRRINO. bmink, if you are going to peck make darn sure to dwell at the bottom to fully break the chip. This will save much nashing of teeth. -matt

TRRINO · Dec 20, 2007

I'm feeding at .0003 but it's mostly to get the depth I need.You could push that a little bit in the 6061. It's softer then my 6AL4V but the chips look simalar. I run a part that is 6061 with a .043 drill ---.0005 feed @ 7000 RPMs---.300 deep---.120 first shot then .075 after but it's a blind hole no break thru.
In our Titanium with that depth we use high pressure coolant but at a low PSI--it will deflect the drill. I would say you wouldn't need to start slow - unless you are not centering before drilling.

TRRINO · Dec 20, 2007

Madlab said:
I have a new Hero...... and he lives in Pa. I have heard M.A. Ford made good drills ... now I have to try some out. 1.25 deep wow........ good work TRRINO. bmink, if you are going to peck make darn sure to dwell at the bottom to fully break the chip. This will save much nashing of teeth. -matt

Hey Matt don't do that dwell on stainless---it'll work harden in the bottom of hole and make it hard to get back in the cut--should be ok in the 6061 though.

Madlab · Dec 20, 2007

Ok, I always try to program a really small dwell when pecking to break the two "strings"
formed by the chip flowing up the spiral. this breaks small drills when you are feeding and pull the drill back suddenly. But you are right on stainlees and small drills. I am going to order some Fords today. Thanks again-matt

bmink72 · Dec 20, 2007

Thanks for the input everyone.

Search

Largest Manufacturing Technology Community on the Web

Search

.026 Dia. holes in Aluminum

bmink72

Plastic

gdgambler

Hot Rolled

bmink72

Plastic

g-coder05

Titanium

TRRINO

Aluminum

bmink72

Plastic

Madlab

Hot Rolled

TRRINO

Aluminum

TRRINO

Aluminum

Madlab

Hot Rolled

bmink72

Plastic

Similar threads