[l u k e]

I'm going to be doing a job that requires a 2" diameter hole, 5 1/2" in length (Through hole). The material is 6061 aluminum.

I have a Boring Head but the longest bar is 3". If possible I would like to avoid boring from both ends.

I was wondering if this bar can be used with a boring head? >>bar<<

If so what would you recommend as a tip for 6061, with or without chip breaker grooves?

Also what lead angle would be best for aluminum, -1* or -5*?

[Mcgyver]

i can't see why you couldn't do it with a boring head, except that a 1/2 bar with 5" of over hang seems like a lot - it'll work but with light cuts and very fine/no feeds cuts before measuring to work the spring out. You'd be better off with a carbide boring bar (less flex) but its still not an ideal length to dia ratio (iirc 5 or 6x). All this assumes the 1/2" comes from the size of bar your boring head will hold.

If the part allowed it, i'd do it in the lathe with a larger dia boring bar.

[l u k e]

i can't see why you couldn't do it with a boring head, except that a 1/2 bar with 5" of over hang seems like a lot - it'll work but with light cuts and very fine/no feeds cuts before measuring to work the spring out. You'd be better off with a carbide boring bar (less flex) but its still not an ideal length to dia ratio (iirc 5 or 6x). All this assumes the 1/2" comes from the size of bar your boring head will hold.

If the part allowed it, i'd do it in the lathe with a larger dia boring bar.

Yea, my head is 1/2" and I don't have a lathe.

Would you suggest just boring it from both ends.

[mxtras]

I recently used a boring head with carbide tipped tooling to bore a 5.25" hole, 1" deep in 6061. I broke some of the rules by raking the bar back by about 3 degrees (a guess) and I honed a small radius (maybe a 1MM radius) on the tip for the finishing cuts.

I started with a 1" drill, then plunged with the largest end mill I had which was a 1.5" rougher. I then hogged material from there manually plunging the cutter in a pretty hap-hazard fashion to get the majority of the material out of the way using a scribed line as a visual reference. Once I got most of the material out of the way I switched to use the adjustable boring head and positioned an old boring bar on the OD of the boring head. When I got close to size, I switched the cutter to a more rigid bar and took fine cuts from there. It took a bit of time, but I had no issues with finish cutting.

This was prior to completing my CNC - now I would interpolate then true it up with the boring head.

Scott

[l u k e]

Yea, thats the same head I have. The problem is the 5.5" deep hole.

[mxtras]

I read right over that without really thinking about the length/diameter relationship - sorry!

Carbide bar or light cuts is all that comes to mind at the moment. I guess a reamer is out of the question (cost).

Another option would be to get your hands on a smaller diameter boring head that would allow the head itself to go into the hole - then you would be set. Something like a DeVlieg boring head as shown below.

What machine are you doing this on? Do you have enough quill stroke?

Scott

[l u k e]

I read right over that without really thinking about the length/diameter relationship - sorry!

Carbide bar or light cuts is all that comes to mind at the moment. I guess a reamer is out of the question (cost).

Another option would be to get your hands on a smaller diameter boring head that would allow the head itself to go into the hole - then you would be set. Something like a DeVlieg boring head as shown below.

What machine are you doing this on? Do you have enough quill stroke?

Scott

I have a manual import, I have plenty quill stroke.

The hole actually has a capped end. (sort of like a U-joint cap on a drive line)
So I do have some room for deflection on the bar. What kind of tolerance might I expect with the bar I linked here?

I'm going to take 2 separate pieces of stock and drill and tap the 2 sides, then bolt them together. Then I'll bore the hole between the two pieces. There will be another part that will be "sandwiched" between them. I can always mill a few thousands off one of the halves if the hole is a little off.

I guess I didn't really give enough information with the original question.

I guess really what I was asking was if the bar was suitable for a boring head and what lead angle and tip should I buy for aluminum? Being new to machining (and self taught) I always assume I'll end up buying the wrong tool for the job....

[mxtras]

I think the bar you have will be fine. For aluminum (right or wrong) I use a positive rake tool with a small corner radius and I use Tapmagic for finishing cuts to improve the finish quality. The bars I use the most are cheapies that have a neutral face so I cheat by grinding a bit more radial clearance and rotate the tip forward to falsely create a positive rake.

For finish cuts, I use .001" per rev downfeed at a relatively slow RPM to eliminate vibration from the cutter being off-center. I am thinking around 500RPM or so.

Scott

[l u k e]

ok, it's sounds right to me, thanks for the info..

[tim-tbl]

Have you tried using an SR bar and cutter mounting that in the quill, however having bored plenty of holes in plenty of metal you could really do with boring the part in a lathe.

[mxtras]

Tim -

Do you have a pic of what you are refering to?

Just curious.

Scott

[miljnor]

well I going to be "that guy" and say the obvious an since you are new.....


Use the force luke use the force!

[Mcgyver]

oh man that hurt. i need a drink now

luke its just the excuse you need to buy a lathe!

ps I'd try in one cut - it would be a pita to get it perfectly aligned AND get the dia perfectly the same.

[l u k e]

oh man that hurt. i need a drink now

luke its just the excuse you need to buy a lathe!

Yea I know, but I'm looking for a cnc mill first, I hope to make a purchase in the next few months, just not sure "who" should get my money.

[Geof]

Be unconventional; figure out some way to mount the workpiece to the mill spindle and hold the boring bar in a vise. Pretend it it a vertical lathe upside down.

[thogib]

If you get a boring bar for a lathe, prefferable carbide and with an insert, that has a 1/2" diameter shank, you can mount it in your boring head. I like the Sandvick bars and most of the tool makers have inserts made specifically for alum.
We've done .3750" +/-.0002" and .6250" +/-.0001" :cheers: bores in the 6" length using this method.
Also don't do a spring cut. Start about .04" undersize; bore, measure, and adjust cut, to cut about .010/side. see how much it actually cuts adjust as needed and go for it. Skim cuts and dead passes on that long of a tool almost always wind up oversized.

[widgitmaster]

I just bored two holes to .8745 that were 4.5" deep using a standard brazed
carbide boring bar with the shank thinned down to give me the extra reach!

I just improvized, and got both bores the 1st try!

Eric

[tim-tbl]

Tim -

Do you have a pic of what you are refering to?

Just curious.

Scott

Hi Scott

Here is the pic of what I refer to as SR bars and cutters

Cheers
Tim

[BobWarfield]

If you are going to do this once in a blue moon, I'd order a couple solid carbide boring bars to fit you head and just go slow. The DeVlieg would be cool if you can find one cheap, but that's not easy. It'd be a worthwhile thing to have around though.

If you have to make very many of them, you could invest in an indexable drill, 2" diameter or close if you feel you want to bore the last little bit for precision.

Best,

BW

[HuFlungDung]

I've never tried this, but if the bar you use is small, and there is room in the hole you are working in, it might work to make some kind of a dampener/brace between the unused hole in the boring head, and the back side of the boring bar. I might try to support the bar about half way down. The idea is to have something there to absorb and dampen vibration of the bar, because usually, once it starts to chatter, it rapidly gets worse. So if you can vibration dampen the bar, then you might actually be able to do it with pleasing results.