[nfrees114]

Hey Guys- So I've been having a hell of a time. I have an aluminum part that I am machining with 8 holes/counterbores that are .170" Dia 1" deep with a flat bottom. tolerance is +/-.002. So I bought a .125" end mill with a 1" deep cutting depth. well I milled it and the hole came out tapered. Like the mill is defelecting a lot..... I've been thinking about this all day and am not sure what the best way to get this to work it. I thought about drilling and reamming it to .170" leaving .025" at the bottom and then clean that up with the .125" end mill. Or grinding the Reamer so it will cut to full depth? but with that i'm afraid it will chatter and be way oversized. Anyways I have 10 of these parts with 8 holes per piece and don't want to scrap anymore parts. If anyone has any ideas i'd love to hear them. I'm getting frustrated... :-)

Thanks guys!
-Nate

[nfrees114]

I should also add that there is an 1/8" through hole that goes into that also. so it's an 1/8" thru hole with a .170" counterbore 1" deep. figured i better add that. so i drilled the hole first that way the 1/8" end mill wasn't center cutting.

Hey Guys- So I've been having a hell of a time. I have an aluminum part that I am machining with 8 holes/counterbores that are .170" Dia 1" deep with a flat bottom. tolerance is +/-.002. So I bought a .125" end mill with a 1" deep cutting depth. well I milled it and the hole came out tapered. Like the mill is defelecting a lot..... I've been thinking about this all day and am not sure what the best way to get this to work it. I thought about drilling and reamming it to .170" leaving .025" at the bottom and then clean that up with the .125" end mill. Or grinding the Reamer so it will cut to full depth? but with that i'm afraid it will chatter and be way oversized. Anyways I have 10 of these parts with 8 holes per piece and don't want to scrap anymore parts. If anyone has any ideas i'd love to hear them. I'm getting frustrated... :-)

Thanks guys!
-Nate

[fizzissist]

An end mill will not give you a flat bottom from plunging because the end isn't ground square. If you do a helical gradual plunge with a 5/32 endmill after a 5/32 pilot drill, you'll still likely get some taper with a 1" deep hole.. Me? I'd do the 5/32 helical bore to a dia of say, .165, followed with a boring bar to size.

If you're going to use a reamer, the ideal would probably be an unequal spaced right hand flute spiral.

To avoid scrapping any more parts, make some tests using the same material and cutting conditions with some scrap material.

[RICHARD ZASTROW]

Try an end cutting jig borer reamer to finish the counterbore?

Dick Z

[Perfect Circle]

Carbide Center Cut and low RPM's the hole should stay the same size as the carbide mill maybe .0005 bigger.

Stop the endmill at the bottom of the hole then retract it without the spindle running =Ive had this prob on other matl. than AL. and the heat from the cut would make the endmill or reamer heat up and poof when you retract it while the spindle is running ...oversize
DONT Climb Cut!
Hope that helps.
Good Luck~!

[PixMan]

1. Drill hole Ø1/8" through
2. Drill hole No.18 (Ø.1695) .990 deep
3. Drill hole No.18 (Ø.1695) 1" with drill modified for flat bottom

HSS drills are dirt cheap and will get the job done. I can modify one to be a flat-bottomed drill in about 30 seconds and it'll work fine.

Carbide Center Cut and low RPM's the hole should stay the same size as the carbide mill maybe .0005 bigger.

Stop the endmill at the bottom of the hole then retract it without the spindle running =Ive had this prob on other matl. than AL. and the heat from the cut would make the endmill or reamer heat up and poof when you retract it while the spindle is running ...oversize
DONT Climb Cut!
Hope that helps.
Good Luck~!

This strikes me as wrong on many levels.

Don't climb cut with carbide? In aluminum no less? Carbide has a distinct aversion to low speed anything.

Using a carbide end mill on this is clearly over thinking. This should be done complete with simple drills.

[ALLtra Mach]

Carbide end mill, all the rpm's you've got, helical with multiple springs and you should be able to hold size all day long.

then go kick the engineer that designed that hole in the nads...6x deep with 15% tolerance....

[M250cnc]

Wow no one got the right answer yet.

This problem is all about cutter flex

So modify the cutter as follows, this only allows cutting at the end of the cutter so that the flex is the same no matter where it is cutting provided the cutter does not leave the hole while engaged.

If i was doing this i could even make the bottom of the hole tapered bigger.

Phil

[PixMan]

I can't understand why you all seem to think this problem even needs milling.

Small-diameter, long length-to-diameter ratio milling is something done all the time, successfully. We don't even know if the machine has the 20K to 50K rpm that these 4mm carbide end mills need to be efficient. But that is not the issue, it's economics, plain and simple.

This is a "pay job". You cannot be making any money on 80 small holes if you are custom grinding carbide end mills and screwing around with tapered helical tool paths. If you were working for me and didn't have this job done in the first 30 minutes with a flat-bottomed HSS drill, you'd be looking for your next job.

[M250cnc]

This is a "pay job". You cannot be making any money on 80 small holes if you are custom grinding carbide end mills and screwing around with tapered helical tool paths. If you were working for me and didn't have this job done in the first 30 minutes with a flat-bottomed HSS drill, you'd be looking for your next job.

Doing it the way i described does not need a tapered helical toolpath only if i wanted a taper at the bottom.

I would agree about drilling but it depends on the tolerance and finish required.

Phil

[PixMan]

Doing it the way i described does not need a tapered helical toolpath only if i wanted a taper at the bottom.

I would agree about drilling but it depends on the tolerance and finish required.

Phil

The OP already stated the tolerance to be +/-.002" (.05mm) so that's a drill tolerance all day long. No finish given, but I'm sure it could be nice with the right drills.

[ALLtra Mach]

I can't understand why you all seem to think this problem even needs milling.

Small-diameter, long length-to-diameter ratio milling is something done all the time, successfully. We don't even know if the machine has the 20K to 50K rpm that these 4mm carbide end mills need to be efficient. But that is not the issue, it's economics, plain and simple.

This is a "pay job". You cannot be making any money on 80 small holes if you are custom grinding carbide end mills and screwing around with tapered helical tool paths. If you were working for me and didn't have this job done in the first 30 minutes with a flat-bottomed HSS drill, you'd be looking for your next job.

And if you were working for me and had to "screw around" with a helical tool path you'd be looking for your next job. I can write the program for that quicker than you can grind your flat bottom drill! I also make holes like this on a machine with an 8K spindle!

I don't believe he ever told us what type of machine he was even using?

Plain and simple fact is there is more than one right answer to the problem.
But there is no need to condemn the way others do things. Phil and I both gave him some more options to use, as did you. You just gave unneeded attitude!

I never use a HSS drill in aluminum if I want an "efficient" and accurate 6X dia hole.