deep drilling small holes in aluminum

[Fremont Dave]

I'm new to machining and am running into trouble. I have 70 .076 diameter holes per part in close packing (.025 walls) going down 1 and 1.25 inches in 6061-t6. I'm breaking drills after about 5 holes. Currently running around 4K rpm using a peck cycle with .075 pecks at 8 ipm. I'm rapiding fully out of the hole and returning .02 short of my last depth for continuing with the next peck. I'm using flood coolany on a Fadal. I was using new parabolic drill bits I got from mcmaster. Didn't see any markings on them. Can anyone recommend feeds, speeds, peck sizes, coolants or drill bits to use. Thanks for the help.

Dave

[dertsap]

a peck should be 1/2 of the drill dia max

your speed and feed sound ok

[jackson]

Originally Posted by dertsap a peck should be 1/2 of the drill dia max your speed and feed sound ok

Yeah what dertsap said, may be make the return after the peck about .05 i usually make mine .1 just cause that is were i am confortable and you could go a bit faster on the rpm but it will work just fine were it is.

[Caprirs]

I agree with the others. The peck is too much for that drill. Most of the parts I do have small holes, although not nearly as deep as what you're running. I would run 6000rpm and 10ipm with a peck of .030".

http://evlgt85.com/gallery/MC_Machine_Samples/sample6

[Eurisko]

Spot the holes first with a short center drill.

As a general rule of thumb, peck drilling should be used when the drill depth exceeds 3 times the drill diameter.

The parabolic .076 drill should easily peck 1 to 2 times the drill diameter during each cycle.

It isn't necessary to rapid completely out of the hole after each peck.

Also, Your feedrate may be a little high for the rpms you're running.

HSS drilling in aluminum, roughly 200 surface feet per minute.
For a .076 drill, that equates to 10,000 rpm.

I'd try .001 feed per rev, ( 10 ipm @ 10,000 rpm )
Or 5 ipm @ 5000 rpm for a more conservative speed.

[Fremont Dave]

Thanks for all the help guys. I'll give cut my step in half and rerun.

[WayneHill]

Use a straight flute carbide drill. Much more solid than a spiral flute drill.
It will last forever in aluminum.

[Eurisko]

Here's an interesting link to microdrilling:

http://findarticles.com/p/articles/m..._n8942198/pg_3

It seems that for VERY small drills, the behavior is non-linear.

Just when I thought I knew it all...

[Fremont Dave]

Thanks again for the help from everyone. I wanted to capture what I did incase someone else comes looking with a similar problem.

I ended up taking a mix of your input. I set up 6K spindle at 10 ipm with .03 pecks using rapiding out to the clearance plane and rapiding back in with a .1 gap before the next cut. Ran 3 parts (70 holes each) with no problems. I bought PTC extra long parabolics. They were TIN coated since that's all the tool supply had but they hardly loaded up with aluminum.

Eurisko,
I did try your setup earlier since it's in keeping with the manufactuer's claims on parabolics but without luck. I only managed 4 holes before snapping the bit despite stopping and checking for chips wrapped in the bit after each hole.

Thanks again everybory.

Dave

[Mitsui Seiki]

Jusr for the heck of it.
I'm using Sandvik Coromant R840-0400-50-A1A 1220.Dia 4mm, drill length 50mm internal coolant,for my alumimum parts. I drill 10 1inch deep holes in each part.S10000rpmF1200mm/m peckdrilling.No problems at all.I change it after every 500'th hole.

[seanreit]

How do you change how high the peck comes out of the hole? I've never seen that option, mine pecks back out to .1 or .05 depending on what I set.

"It isn't necessary to rapid completely out of the hole after each peck."

[Fremont Dave]

Hey Seanreit,
When you say it comes out .05 or .1 depending on what you set, are you referring to what you set in your CAM package? If so, you might have to get into the g-code which isn't so bad or perhaps tweak your post processor which I would pass off to my reseller for lack of time. The few CAM packages I have played with allow me to set my clearance plane height which sets the distance you are asking about. For me, using my FADAL, a deep cycle looks like the following:

G83G99X0Y-2.325R0+.1Z-.736P.02Q.1F5.

The cycle starts with the G83, G99 calls the cycle back to the initial plane which is flagged with the R0. Right after that it Z's up .1 which is where I set my clearance plane. If your not on a Fadal, I'm sure it'll look different but that's all I can speak to. Like I said in the begining, I'm pretty new to machining.

Dave