Thread: Boring setup advice

Hi guys,

I’m going to start working on a job next week that requires boring a little deeper and larger in diameter than I’ve done in the past and would like to get a little input and advice.

The material is 6061 T6 4.25” dia x 2.25 long. The bore is 3.35 dia to 1.0” deep then narrows to 1.375” the rest of the way thru. I’m planning to drill a 1-/4” thru hole then bore with a 1” bar.

I have 200 of these to do so I would like to get an efficient setup the first time. The T32B programming manual describes an alternate boring cycle called “inside diameter deep hole dividing cycle” which basically allows thru parameter U35 to control the depth in Z to help chips from clogging up in the bore. Is this a good choice or just a waste of time for this part?

I’m thinking of using 1200SFM with a DOC of .1”. Is this a little light in DOC for roughing with a 1.0” boring bar in 6061?

Any input or advice would be appreciated.

1: I'd go with a 3/4" bar (( If my noodle serves me correctly, a 1.0" bar requires a minimum hole of 1-1/4" diameter, which is exactly on size to your drilled hole, it may gall up on you and hit the other side of the hole on the retract move on the "X" when coming out of the hole. 3/4" bar will be fine, BEEN THERE / DONE THAT MANY TIMES. *Go with 2.5" overhang for clearance on the face of the part! ))

2: I'd program a straight "I/D Boring Process" (( Forget about the "U35" Parameter ))

I use a Dcgt insert and .75 bar for aluminium breaks the chips great no packing 1700 and .014 feed works great

You could do it many ways depending on the tooling you already have. If you have one of those monster allied spade drills you could drill to 1.35 and then rough and finish with a 7/8 boring bar on the inside hole but I would do the inside hole secondary to the larger hole so your not finishing the inner bore before you cut out the larger diameter. It almost looks like a 2-3 minute part depending on the speed at which you want to puch things. We puts a little slower in our shop and wont cut more than .15 with a boring bar at one time (1") and at about 2000sf.

The only large boring bar I have is a 1" TPG. Looks like I need to pick up another. I'm not real failure with the styles, lead angles and inserts for boring bars so could use a little guidance in finding what I need for this job and can be also be used for most other boring that will come along.

I was looking at this bar: http://www.carbidedepot.com/detail.aspx?ID=19817 or is there a better option.

What inserts grade would work best on 6061?

Thanks for you input.

Do you have a 3/4" bar? Or a 1/2" carbide?
*The one off of your link is a profiling bar, I'd use it for finishing but not for roughing, furthermore, that style bar in 3/4" shank requires a 1-1/8 min drilled hole, while it is true that you're pre-drilling with a 1-1/4" drill, this bar robs you of a lot of chip clearance, I'd go with a bar like this one:

Nice TPG insert, good chip breakers, 6 cutting edges per insert. I believe a 3/4" bar in this style only requires a 7/8" pre-drilled hole, and being that you are pre-drilling to 1-1/4" diameter, the chips will just fly out of the hole!

I have tons of 5/8 left handed bars that I use for OD work on gang tool lathes and small 3/8" solid carbide tools. The 1" TPG bar I dug up out of an old box of tooling that has been around for years. There was also either a 1/2" or 5/8" trigon right handed steel bar (1/4" IC?) that I found but have to check the size when I get back next week.

Found a right handed 5/8" trigon bar in a box that works perfect. Used 1800 SFM, .075 DOC and .012 feed and nice crisp chip flow. Ended up leaving only .001" for finish on Z otherwise I was getting chatter on the face of the pocket. The 1" bar would have been a problem in that 1.250 hole!

2 Minutes on the money for the first op, 50 seconds to face and profile on the other end. Sweet!

Is there a way to put a Radius on the end of the boring op (the 1.375 dia )to eliminate the need to use the boring bar on the second op? Can you put a -.050" in the final corner line? OK, I'm to chicken to try unless I hear from the professionals!

Sorry about the size of the pic.

Yes Captdave, you use a "Grooving bar" and program an I/D Groove

*It will take a lot longer than just breaking the corner on the second op., once before you used what I recommended for you on the o/d of a part at the end of a taper, use the same process on the I/D of this part on the second side, it will take a few seconds.

SteelCutter<====Not a PROfessional, just too many hard knocks, that's all

Happy Cornering
ps: can you get away with just breaking the I/D by hand on the second side, say with a ROTO BURR aka SUICIDE KNIFE by many, or something like it?

No, it calls for a .050" R so I guess I'll just do it on the second op since it's running well. I would probably waste more time trying to do something different then it currently takes. Oh well I thought it was too easy!

Just pop in a ID groove with a radius and your done dont waste your time on a 2nd Op. If you dont try you'll never gain the confidence it only gets easier after that.

Casvin

I wouldn't have worried about the larger boring bar with a minimum bore the same as the drilled hole because its a thru hole. The chips have some place to go. Then set the TPC to a small retract so it doesn't hit.
We also set our boring bars to use thru bar coolant to help that.
Getting the radius on the far side to match might be hit and miss if you do it from the front, before the other side is faced. It isn't that much time is it? More than what you will spend doing it from the front?

After my 5rd run of 200 of these I started looking for an indexable drill to speed these up a bit. Came accross a good deal on a 1.120" drill (the largest they make in 1" shank) from Ultra-dex for $109 with coolant thru and a port on the side of the shank. Sweet tool, 950 SFM .005 IPR and it plows right thru even though I'm drilling deeper then the recommended 2X. Now using a 1" boring bar and added 2 more set screws on the holder as I was getting a little squeal on the finish pass.

After a little more tweaking, the part now runs 1 minute flat as opposed to 2 minutes with a 1.25 drill pecking.

Very nice. Congrats.