Deep hole drilling

[Veracity]

Former Moldmaker getting into production machining. What is the best approach to drilling a 7/16 hole 3.635" deep in 6061 with a CNC that does not have thru spindle?

I know that its going to be a peckdrill cycle (im assuming) but what should my pecks be once im past 5XD? Or is there a better drill alternative?

[Delw]

Thats not that deep. depending on the drill I would use .100 pecks maybe .2 but .2 will grab lots of chips and may gall up. one very long drills I go slower in the rpm sometimes by half of what is recommended.
For alum deep holes, ( your not going to like this) I buy cheap extended length bits with NO SPLIT POINT, ( those black ones with the real strong not looking like it will cut point.)
they dont walk and they hold size and pull our a better finish than high quality cobalt drills. I have no clue why but they do.

I get them at the local nut and bolt place for a few bucks.
in steel they dont work worth a crap but in alum for deep hole drilling they do a great job.
Also make sure you have plenty of flood coolant, you may have to extend one line just for the drill.
if you dont have coolant of anykind your going to be **** out of luck and be down to .025-.05 pecks at 500 rpm or less.



Delw

[lesr]

Veracity

You could have a look at EditComm, it allows you to produce expanded code very quickly that reduce the depth of peck eah peck with dwells to allow coolant to flush the swarf out of the bore, url below.



regards

Les Robbins


EditComm - CNC communication software - Les Robbins CNC Services

[Veracity]

I've been trying to find this drill with no split point. Still a little confused as to what im looking for.

lesr, thanks for the link. will check it out.

[78nova]

We mainly use Fullerton 3-flute drills for all of our aluminum drilling. These drills have a 5-axis grind and are self centering. For a .4375 drill, I would suggest you start out at 1500 rpm, 10 ipm with a .150 peck. If this works out you can always increase feeds, speeds & peck depth to obtain your best fit for the conditions you are working with.

With the best fit feed & speed using these drills you can obtain a very good finish. We use these type drills to prep for all of our gun drill holes and we also use them in applications like you described.

These drills are a little pricey but you get what you pay for. A lesser quality drill would work, it just depends what you want the holes to look like and how long of tool life you expect for the tool being used.

One of these Fullerton drills will have a pretty long tool life if used properly.

Check them out at Fullerton Tool Company - Solid Carbide Cutting Tools | FullertonTool.com

Good luck!

[Veracity]

A 3 flute for deep-ish hole drilling. Humm, i never would have thought it had enough flute to evac chips properly. But if you say that you do it, i shal give it a try.

[78nova]

If you have not visited the Fullerton site yet I did forget to mention that these are Solid Carbide Drills. A .4375 standard length drill is going to be 4.5" long with 2.875" of flute. It could be modified slightly to get to the depth you need with no problem or you can just order a longer drill that they offer.

With the right conditions a drill this size could also be ran at 2-3 times the feed, speed & peck amount I suggested as a starting point.

We have one job we use a Fullerton .1875 drill on that we run at 4500 rpm, 22 ipm & drill .500 deep with no pecking and we are holding +/-.001 for two tooling holes.

These are really good drills and the tool life is excellent. Many of the jobs we run have Fullerton drills that have ran hundreds of holes.

We mainily machine using 7075 & 2219 aluminum alloy.

[BKGUY]

I would go with a Parabolic Drill from Titex if you don't have coolant thru. They have a very slick finish in the flute gullets and help evacuate the chips. Definitely have to peck every .1" to .2" and get as much flood coolant on there as possible.