PLEASE HELP: See attached pic of folded metal chip

Italiano83 · Sep 25, 2017

So I'm drilling 6061 bar stock on a turning center on the centerline with a .625 diameter drill to a depth of 1.25". Drill point angle 140 and solid carbide drill. Hole looks beautiful, no issues there. Then I come behind the drill with a .375" diameter solid carbide boring bar. I need to bore to .827" diameter, .750" deep. I've reduced the DOC to .030" just to see if light cuts would help, but no it doesn't. I'm getting this folded piece of metal in the back of the hole that the next pass grinds against and can't figure out why I'm getting this. See the picture I've attached and the simple code is something like:

G00 X.685 Z.1
G01 Z-.750 F.003
X.600
G00 Z.1
X.745
G01 Z-.750 F.003
X.600
G00 Z.1
X.805
.....AND SO ON UNTIL A .827 DIAMETER IS REACHED

mhajicek · Sep 25, 2017

Looks like your insert may not be sharp enough; is it a polished, razor sharp insert for aluminum or a general purpose insert? If you don't have a better insert available you might try boring the other direction; pulling instead of pushing.

Italiano83 · Sep 25, 2017

No Insert. These are brand-new solid carbide boring bars. The problem with pulling the initial plunge up into the material is going to be nasty, especially since it would need to be at the very rear of the hole, so that's at max hangout position.

Bluejeep · Sep 25, 2017

Maybe not enough end relief or underside relief on the boring bar. looks like its not making a chip and just plowing material. I would double check that the business end of the boring bar is set on center. if those don't end up being the problem then buy this bar with some inserts for aluminum. 1/2" STEEL SHANK BORING BAR and run your passes the same except dont bring your X back to .6 (bar is to big for that) until you bored out enough space.

mhajicek · Sep 25, 2017

Who did you get the boring bars from, and what part# are they? I can guarantee you from looking at that chip that they were not designed (properly at least) for aluminum. You need a very sharp edge with proper relief; different geometry than for cutting steel. An edge designed for steel will just shove aluminum around like you're seeing.

Bobw · Sep 25, 2017

Those flat top little bitches from Micro 100???

They work, but the geometry (WHAT??? Geometry) Fricken sucks..

Its like using a TPG insert from the 50's..

I haven't bought one of those little solid guys in YEARS.. Just use a beat
up old carbide endmill. Its going in the scrap bin anyways.. Just touch
it up, maybe some clearance, and let it rip.

If you insist on using it... Get out the green wheel and the diamond file..

guest · Sep 25, 2017

Italiano83 said:
No Insert. These are brand-new solid carbide boring bars. The problem with pulling the initial plunge up into the material is going to be nasty, especially since it would need to be at the very rear of the hole, so that's at max hangout position.

If you have an ID grooving bar you can go in and make some space at the bottom of the c'bore. Might have to take it in 2 passes, groove to .725, bore to .725, go back in and groove to .825 then finish with the boring bar.

But I'd lose the solid carbide bar and get an indexable in there. Better chance of pulling the chip out of the hole instead of pushing it in front of the tool.

I agree with Bobw- an old endmill will work just as good as that boring bar. Hell it's aluminum- you can plunge a 7/8 2-fluter in the hole on centerline and just use the boring bar for the finish pass.

edit to correct: meant to say 13/16 2-fluter- not sure why I had 7/8 on the brain...

brian.pallas · Sep 25, 2017

I've ended up just programming in a chip break for roughing any aluminum, especially 6061. Semmed like we were always chasing the chip issues. Programming the chip break was the most reliable way of doing it. Doesn't take long to do it by hand.

(Also it is nice the MCam added in that specifically. I had been using the tool inspection to get what I wanted sometimes, but the change they made made it easier.)

But I'd still do it by hand if needed. Leave like .005 or .010 a side, rough it with a peck, then finish the bore. We always used a .050 peck, then back off .015 I think it was. It mught need more retract though. Just use U and W incremental moves for your peck.

But +1 to an endmill also.

Tonytn36 · Sep 25, 2017

Agreed with the plowing. As noted, make sure there is end relief on that bar. But for .75 deep, 2 flute end mill and be done.

Bluejeep · Sep 26, 2017

Another thought, is the spindle rotating the right direction?

david n · Sep 26, 2017

End relief on the boring bar and...................material mill? Is this domestic Ali? Or some no name Chicom garbage?

Dave K · Sep 26, 2017

Bluejeep said:
Another thought, is the spindle rotating the right direction?

I would think he'd have more problems than just a folded chip if it were running the wrong way, no?

Search

Largest Manufacturing Technology Community on the Web

Search

PLEASE HELP: See attached pic of folded metal chip

Italiano83

Aluminum

mhajicek

Diamond

Italiano83

Aluminum

Bluejeep

Hot Rolled

mhajicek

Diamond

Bobw

Diamond

guest

Guest

brian.pallas

Hot Rolled

Tonytn36

Diamond

Bluejeep

Hot Rolled

david n

Diamond

Dave K

Diamond

Similar threads