3/8 hole ~9D deep in 6061

gustafson said:

How many do you have to do

I guess I would center drill then drill, to keep the wander down. might be tempted to go most of the way with a stub drill to keep it straight, but it is another tool change, which is time

Click to expand...

DanielG said:

I'm only doing two of them. Unfortunately though, this hole is drilled fairly late in the process, so if the hole is bad, a lot of work is wasted. So I don't really care how long it takes to drill the hole, just that it's right.

Click to expand...

DanielG said:

I'm only doing two of them. Unfortunately though, this hole is drilled fairly late in the process, so if the hole is bad, a lot of work is wasted. So I don't really care how long it takes to drill the hole, just that it's right.

Click to expand...

DanielG said:

It doesn't, however, give speeds and feeds for regular aluminum, just for cast aluminum.

Click to expand...

Bobw said:

You are way overthinking this...

First. You have a tolerance after anodize of 378-381.. Why are you reaming it
right in the middle when there is going to be buildup.. Go for the high side.
Then you don't have to worry about it.

As for drilling it.. Just drill it. I do a ton of expensive castings, and I just
take it easy.. Where I could punch a hole at .010 a rev if it was just a piece of
cheap ass bar stock.. On something that has some money it in already.. Take it easy,
make sure that sucker comes out straight. I'm not going to run max surface speed,
and max feed to save 30 seconds, when I could take 2 minutes to do it and make 100%
sure I don't toss $750 casting in the trash.

I would definitely use a split point. A jobber is almost long enough to get you through,
Grind a little relief at the top of the flutes, and you'll have enough length. I'd keep
the surface speed conservative. Maybe 120-150, and the feed at about .003 or .004 a rev,
depending on how I felt that day.

To start the hole, a stubby drill, split point of course.. You could even use the jobber,
just feed her in about .100" at .001 or .0015 a rev or so..

As for the reaming.. Again.. I play conservative. On something that is going to cost me money
if it goes oversize, I run 'em slow, and I get very consistent results. My go to on things I can't
screw up is about 240 rpms.. Regardless of size of reamer, or material.. I'd probably be feeding
at about .005 or .006 a rev.. And yeah, that's slow.. But it will be consistent..

I know that all sounds SLOW.. It is.. If its a $4 piece of bar stock, and I have 100 of 'em to do,
wind it up and punch it. But when the part already has a ton of work into it, or the material/casting
is going to cost an arm and a leg to replace.. Those are my GoTo #'s.

I'm also a huge fan of taking a test cut on a separate piece of material that is similar.. Make sure
your hole making technique is going to give you the results you want.. Even if you just punch a 1x2"
aluminum soft jaw the 2" direction as a test.. You'll know its going to work, and you're out 5 minutes.

Click to expand...

DanielG said:

I need a thru hole in 6061, about 3.25" deep, to be .378 -0/+.003 after anodizing. My anodizer says I'll have about .0006 per side, half of that being buildup, so I was going to go for a .3795 hole before anodizing. My current plan is to spot drill, then drill 23/64 thru from one side with a good taper length drill, then ream with a .3795 reamer with plenty of cutting fluid. I can do the reaming in the machine (should I have a special holder for this?) or with a hand drill or drill press.

I did think about drilling from both ends and then reaming through, but my concern is that they won't be perfectly concentric and the reamer will follow a wandering path.

For the drill, a Guhring 535 series is readily available. It looks like a good drill and says it's good for non-ferrous and steel, just not stainless. It doesn't, however, give speeds and feeds for regular aluminum, just for cast aluminum. That seems pretty common and confusing. For example, the 5536 says on it's page that it's good for non-ferrous, but then the non-ferrous section is blank on the speeds and feeds document.

It looks like the best drill for aluminum might be the 501, but it's just for non-ferrous. I'm only doing two of these parts, so if I can buy a more versatile tool and use it again on another project, that would be great.

Click to expand...