What's new
What's new

Good way to Bore A LOT of material w/ Minimal Passes on Lathe ???

Italiano83

Aluminum
Joined
Mar 4, 2013
Location
Miami, FL
So...we typically deal with small aluminum mill-turn parts here of less than 1" diameter. However, we have a new program for parts that are about 2.5" in diameter and have thru holes anywhere from 1.5" to 2". Obviously we can use a fairly large drill 1" diameter or so, and bore out the rest with a large boring bar. But even still, for high production (1000+ pieces) I'm maxing my boring bar out at .100" DOC, so SEVERAL passes are required. What other tools can be used? Finish is not super important. Big twist drills are pricey and we'd have to get them with reduced shanks to fit in our collets. Any recommendations?
 
So...we typically deal with small aluminum mill-turn parts here of less than 1" diameter. However, we have a new program for parts that are about 2.5" in diameter and have thru holes anywhere from 1.5" to 2". Obviously we can use a fairly large drill 1" diameter or so, and bore out the rest with a large boring bar. But even still, for high production (1000+ pieces) I'm maxing my boring bar out at .100" DOC, so SEVERAL passes are required. What other tools can be used? Finish is not super important. Big twist drills are pricey and we'd have to get them with reduced shanks to fit in our collets. Any recommendations?

Insert drill is what you want. Depending on the machine you can go all the way close to your final bore size with the drill. Will need to be mindful of coolant and chipload, but that would be my first step. I have a recurring job making 1-3/4" holes 4-3/4" deep in 6061, and a 1-11/16" insert drill works a treat.

Regards.

Mike.
 
ive been using Quad turn tools for a while, its a drill and a boring bar in one, not only do you save a spot on the turret but it can take depths of cut half the diameter of the drill (depending on the machine).

with my 25mm one i can get 50mm bores in 2 passes.

Link
 
Adding onto what pmack said, a flat bottom insert drill about 1.5 in dia. This one tool can do the whole op. It will punch the hole, then bore the hole out. I have one and it will handle .200 D.O.C.
at around .005 to .006 inches per rev.
 
Ok, I'm pretty new to machining (only a few years experience), so I've never used an insert drill. But I have like $4k left on a Kennametal tooling cert that I have to use by the beginning of March before it expires, so this will be a good opportunity for me to include some with my next purchase. Thanks everyone!

-Jon
 
+1 on insert drill...and you can offset them X and use as a boring bar after the initial hole drilled
 
Insert drill. Buy the biggest one that will fit in your parts, and stuff it in fast.

This is going to sound like a "Jerk" thing to say, but if this job really matters, save yourself some money (long term) and burn that tooling certificate, and get a Seco Perfomax, or Sandvik Coro-Drill 880 insert drill. Seriously. Those drills, and maybe a couple others will blow away the Kennametal drills, both on performance, and tool life.
 
Bigger drill, bigger bar. It depends on how much money you want to throw at it. You could get by with an 1-3/8 (or whatever is about 1/8 to 1/16 smaller than finished I.D.) HSS drill, shoved through scary hard, followed by a 1" CNMG boring bar at .200 per side or whatever you have left, sans a finish pass if needed...

At those quantities, it most likely would be prudent to go with a drill/bar combo tool. But, it all comes down to how much time costs for you...

If you save five seconds per part with a combo tool vs. a far cheaper drill and separate bar, that still only comes out to about an hour and a half saved over 1000 parts... where I work, that comes out to 90 bucks in shop rate. Not really enough to cover a fancy insert drill. But, if it repeats, you'll make it up.

Depending on material cost, though, as the above poster said, it may be yet more efficient to start with thick-wall tubing. No need for a drill at all then, just hog. Only issues might be delicacy in clamping and dealing with ringing.
 
What is the machine you will be running these parts on?

Okuma Genos L300MYW. Big turnmill with some balls. I'm going to go with the insert drill. We barfeed everything here and buying tube stock becomes an issue for the pusher (sometimes) when loading a new bar. Also, like I said, I have free money from Kennametal that I need to use and regardless of others opinions, kennametal makes some darn good inserts for their tools. I especially like their Novo software which gives you feeds/speeds/DOC for all types of materials based on the tooling chosen. We do some excotic stuff here on occassion and their calculations have been spot on (recommended starting points anyhow).

-Jon
 
+1 on insert drill...and you can offset them X and use as a boring bar after the initial hole drilled

actually, you can start the hole oversize, tool offset from center... sounds crazy but it basically bores and drills in the first go. I use that to punch the hole to a specific "sweet spot" roughing size in a single plunge (which can be above the insert drill diameter), then bring in a boring bar for a single finishing pass to size.
 
We run some parts like this and I normally use a 3/4" solid carbide through coolant drill first and then switch to a 2" inserted drill to rough the hole out. The machine is happier sounding and I can run much faster than by just using the insert drill. Cycle times end up being the same so nothing lost there. This is on a little Genos L200EM, so a little smaller than yours.
 
Personally I like the Kyrocera EZ turn indexable drills...they cut with so little pressure compared to other brands...nice for alum as chips just flow ez. But they are all good.


As to tubing...
Yes, barfeeding can be an issue, need to make end plug and hope it doesn't fall out.
Could also use Bar puller.

Other down sides-
Coolant flows through and can get very messy.
Sometimes tubing I find softer or gummier.
Chips go down the tube and come out at the worst times.

Price up-charge for tubing can cost more then popping in a hole.
 
So...we typically deal with small aluminum mill-turn parts here of less than 1" diameter. However, we have a new program for parts that are about 2.5" in diameter and have thru holes anywhere from 1.5" to 2". Obviously we can use a fairly large drill 1" diameter or so, and bore out the rest with a large boring bar. But even still, for high production (1000+ pieces) I'm maxing my boring bar out at .100" DOC, so SEVERAL passes are required. What other tools can be used? Finish is not super important. Big twist drills are pricey and we'd have to get them with reduced shanks to fit in our collets. Any recommendations?
.
.
Allied Spade (Original T-A) drill works fairly good. the holder will fit different size inserts for different diameters within certain size range. they have newer types that are better but the T-A still work ok .
.
like any drill hp is a concern. just cause you got a big drill does not mean your machine can handle it. T-A spade drill inserts are available in HSS and Cobalt.
.
Carbide is good in smaller sizes but over 1" dia and often machine does not have the hp to run the drill
 
Okuma Genos L300MYW. Big turnmill with some balls. I'm going to go with the insert drill. We barfeed everything here and buying tube stock becomes an issue for the pusher (sometimes) when loading a new bar. Also, like I said, I have free money from Kennametal that I need to use and regardless of others opinions, kennametal makes some darn good inserts for their tools. I especially like their Novo software which gives you feeds/speeds/DOC for all types of materials based on the tooling chosen. We do some excotic stuff here on occassion and their calculations have been spot on (recommended starting points anyhow).

-Jon

How can you be maxing out your d.o.c. at .100" on this machine?? It can handle quite a bit more than that!
It's aluminum, get the biggest insert drill for your part (NOT SPADE). Get aluminum-specific inserts for your bar and drill. And get a boring bar that allows you to take a friggin cut! :P
 
How are insert drills on breaking chips? I never used one I hate the long thick stingers coming from standard twist drills on 6061 so for the OP's case if I can't use pipe or tubing I will just feed the hell out of an insert boring bar that has edge geometry conducive to chip breakage. If you get good quality 6061 and not gummy Chinese crap you can go insanely high SFM on a lathe if you have the horsepower and a good hold of the part. I used to make center sections for custom alternators back in the Dualkit days. I would bore out the inside of a 7" diameter chunk of 6061 at 3,000 rpm to a diameter of 5.50". I thought the chips hitting the window were going to break it.
 








 
Back
Top