Lathe drilling .700" hole in 6061 Al with thin wall

[viper]

Per another thread, I had changed the direction of my thread so thought I would just start a new one. There is a pic of the part in the other thread

http://www.practicalmachinist.com/vb...ol-191823.html bottom post has the pic and desc of operation

I would like to drill this hole with just the drill to finished size without reaming or boring if possible. I have never reamed with the lathe because a bore bar makes more sense and leaves a better finish. I am thinking above all, I would need to consider through coolant to get a good finish. I am just thinking that chip clearance and evacuation would be paramount to do this op properly. I am only asking because I have yet to ever run a center hole on the lathe that does not get a boring op but because of the thin wall and 2" length, I am wondering if the bore bar will just cause issues and the bore size is pretty open so I can just select a close size drill and role on.

[Hdpg]

How do you define a 'good finish'? A new split point drill in 6061 will give you a hole within +0.005" on its size and the finish will be smooth to within a few thou. Two inches deep on 0.7 dia (45/64"??) will only need three pecks and you might get a little witness mark where the drill stops and starts; I don't think through coolant is essential although that would allow the hole to be done in one shot.

The biggest problem is the wall thickness. I find that if the OD is done first the pressure from chips when drilling swages the walls out and if the drilling is done first turning the thin wall is chatter prone.

[viper]

I think you understand my problem. Drilling with such a thin wall could prove a problem. However, drilling first will make a thin wall to deal with on the OD turning so kind of a catch 22. I was thinking if I had an insert drill with a bunch of chip clearance, the chips would not pack and screw up the walls of the part.

The finish is not called out but I know I have rarely made a hole in 6061 with a split point that has put a smile on my face and I think it is mostly due to dragging the chips against the wall on the way out and it has a smeared appearance.

I am not familiar with insert drills so I guess I am just hoping they would do the job but might just try a very high quality HSS drill first and see how things go. Or even grind some of the flutes off so they are not contacting the part and dragging chips. Never tried that but just a thought since that is pretty much what insert drills do. The head is bigger than the flute diam so there is clearance...

[Limy Sami]

My way would be;-

Do the bore thenm/c the OD reduces if not neglegates any chance of vibration & chatter.

Big #'s, talk to the tool co's and get a demo before parting with $$$

Small #'s, twist drill & single point bore.

Thought;- a double tool holder - drill on centre line bore bar in 2nd outboard hole - drill hole, retract, move to bore bar and cut,......... no turret indexing.............. match drill and b'bar lengths to minimise movement therefore time.

[viper]

Thanks for the reply. I agree that the bore bar would get the hole cleaned up and to size but really thought if I could run the drill as a second op, I would not have to worry about rigidity concerns on the OD turning. This is why I was thinking about drilling last and only drilling with no bore op.

Do you think drilling this last would be a disaster? I know doing something like this on the mill would work fine but spinning the part changes things...

[Tonytn36]

I'd be really worried about the drilling pressure flaring the OD with that thin of a wall, if you do the drill op last.
I'd do the drill first, use an undersize insert drill and do a clean up bore with the outside drill insert if needed. Then do the OD work.

[Hdpg]

Originally Posted by viper

......Do you think drilling this last would be a disaster? I know doing something like this on the mill would work fine but spinning the part changes things...

I think drilling last has a good chance to be a disaster. Even on a mill I would not try drilling a hole with such a thin wall; I would drill .2" undersize and then do helical interpolation.

How many of these parts are you doing? For lots and lots of something like this I would make a multipart rotating fixture that clamped on the full diameter in the center and then finish both ends OD and ID in the mill. Similar to the part below where I 'turn' and tap both ends of a part in one mill operation rather than two lathe operations.

[Limy Sami]

Drilling last?.......... probably not, single point boring? very likely. either way with a 40thou wall vibes will be your enemy.

OD turn 2nd?......... depends how you're going to go about it,........... planning the cuts to leave metal to provide as much support as possible will make a big difference.

OK you could sail through it, BOTOH it might be a case of suck it and see.

[DigiSnapMark]

Just did something like that yesterday... drilled then bored, the cut the OD down to size. If you start with plenty of excess OD, then take a good depth of cut, you can turn it down with no problems. I did run a couple finish cuts on the OD, and my gawd it was loud!

[viper]

What were your dimensions and material? My plan was to do the front OD complete by running a couple roughing cuts, then a finish pass over about 50% of the part, then move to the back and run everything but leave enough for a healthy cut off, then do the ID, then cuttoff. I suppose if I have too much torsional force with the drill op, the part could snap off and stay on the drill.

I will have to do some scratching and talking on this part... Just trying to find the fastest way to do it.

Numbers are not that great but using this as a learning opportunity again. I like to try new things and see what I can get away with...

[Hdpg]

Originally Posted by viper

.....Numbers are not that great but using this as a learning opportunity again. I like to try new things and see what I can get away with...

You have a VMC, yes?

Do them in a vise. Bore aluminum softs jaws one hole to take the stock diameter one hole to take the finished OD.

Put raw stock in its hole and machine one end complete.

Make accurately fitting plug for support and grip finished end in its hole with plug inside and finish second end.

Once you are running a complete part comes out every cycle.