Need Help!- Aluminum part off issues.

[bob1112]

I am parting 1.50 diam 6061. I am using some GTL-3 inserts on a blade by imco. grade is IC20. Width of the insert is .120, width of blade is .095, speed does not matter, feed does not matter. The finish, every time comes out looking like lunch meat. Coolant is 6%

I have NEVER been able to obtain an acceptable finish when parting. The finish looks smeared like severe rubbing. I blued up the blade and nothing is rubbing on the blade so must either be the insert or presentation to the part.

Can anyone offer advice in determining what the issue is here?

Example in my program today was 700sf, .003/rev feed, lunch meat. I am now must making test washers as I work through this problem. I know the turret has shown to be a few though off center but I cannot imagine a few thou causing excessive rubbing like this. I can provide a pic if that will help the matter.

Thanks!!

[flyinchips]

Too high? Check the face of the insert.

[bob1112]

I was just inspecting the CL and to be honest, I cannot see that it is off center at all. However, I know the turret is slightly off and the insert, to me, seems settled down in the blade too far. I just learned of the flat stock test pinched between the insert and bar but to my surprise, it did not look bad at all. Pretty much normal to the X CL.

However, I have heard that running slightly above CL is the better way to go. Not sure. Something needs to change though.

[fizzissist]

The cutoff tool being on center DOES matter, and if you can find an insert for that holder that is uncoated with SHARP edges, not the slightly dull/rounded or honed edges that are standard you'll get better cutting action.

Do you have the blade as far back into the holder as possible so it's not over extended and as rigid as possible? Is the blade perfectly straight in the holder? Are you taking a depth cut not over .2 dp per pass so chips are clearing?

What does it look like if you take a kiss pass on the face of the bar so you can see what the cutting action looks like on that side at least?

700sfm on aluminum is actually pretty low, so you're ok there... But I've found that often .003"/rev works out to be a little heavy, despite the recommendations. I usually back off to about .0015-.002"/rev.

One trick you can use that should help a little is to take your passes to about .3"dia (depends on how much mass there is to the part) at maybe .005 PAST the required -Z, then move the tool .005" in +Z and "back face" the part till cut off, actually slowing down the RPM when it comes to the .3 dia. so the part doesn't fly.

6% shouldn't be a problem, assuming a typical good grade of coolant. Personally, I keep it at about 10% just 'cause.

...oh yeah...running .001-.002 above CL is usually no problem. With alum, you generally want to be on or slightly above CL. It don't care for negative rake usually.

Good luck. Cutting off is an art.

[bob1112]

Not sure what you are saying about the "passes". I dip in about .25, back up to knock a small rad in the edge (knock off the burr), and take it home in one pass basically. Do I need to allow clearance in there for some reason?

Update: I ran a test and did a face cut half the width of the insert and it still leaves a junk finish. Looks like the insert sides are dragging on the part and the sides are not sharp. The inserts are old Imcos that are uncoated, ground, IC20. Should be good for this but.... I am now wondering about insert mods to stop all this rubbing... But I am concerned that might change the chip forming and really screw things up.

[fizzissist]

This is what it should look like...

Parting Off Geometry Demo.wmv - YouTube

Parting Off Geometry Demo.wmv - YouTube

This is what it shouldn't look like...

Parting off.wmv - YouTube

Parting off.wmv - YouTube

[bob1112]

I keep hearing people say feed harder. I am running 1000sf and clamping spindle speed to 5000. Feed at .003/rev. I am told to go harder with the feed but.... With all this rubbing, I am concerned about that.

[fizzissist]

One of the problems with parting is that you're cutting on the face, but scruffing on the side.. building up heat. With the heat comes expansion of the parts... creating more heat... That's why the rpm sometimes needs to be lower, along with the feed. Depends on the parts, and if you can get good coolant flow with chip clearing.

Can't help but feel that your troubles are the cutting edges' sharpness, seating of the insert so it's solid, and rigidity..... all the while assuming your aluminum is T6??

[bob1112]

Yes, material is T6. inserts are uncoated and ground. I experimented by hand grinding a little off the sides of the insert well behind the cut edge. That helped and I was at least able to run parts. I have people telling me to go faster, some say slow it down....I dunno but I am set at 1000sf and .004/rev so maybe I should try slowing WAY down and keeping the feed high and see what happens...

On about 1/10 parts, it would cut a convex in the part of about .015 high on a 1.6" diam part. I have got to figure this cutoff issue out... Frustrating... Everything else runs flawless, but cutoff........

[fizzissist]

If you're getting convex/concave cutting, something's very wrong with your tool.
I've cut off alum parts all day long with a H.S.S. Empire P5 cutoff blade, 15deg face angle on a cam screw machine with flood oil and no problems. No constant SFM, relieving passes, nothin'. Just straight in on 1.5"dia till it falls off. Back of the part was never a 32 finish....but reasonable and FLAT.
(face relief angle of 15deg, side relief angles of about 3-5deg, top hollow ground)

Something isn't rigid. Your blade is hanging out too far from the holder, the insert isn't seating properly in the blade and the blade is worn or warped, the blade/insert is not perfectly straight vertically, the ways are sloppy, the material is NOT clamped sufficiently in the chuck...
1 or all of the above.

Something critical on stock that big is that your bar feed MUST be perfectly aligned with the spindle, or the stock can creep in the collet, even chuck... this is worth double checking. This bit me in the ass for the longest time with trouble holding Z tolerances...

... one other thing.... Your insert width should be fine... BUT.... maybe you just need to go up the the next width. It shouldn't hurt anything but your wallet.

[bob1112]

Well, we can work through the list here and see if something stands out.

1. Solid box way machine with .0002 lash in both axis.
2. Has 3 jaw but jaws are worn causing unrepeatable runout but should not be an issue unless flipping a part. Clamping force is no problem.
3. Bar is 1.625 which is max cap for machine. Bar can move about .125 at the tail of the 40" bar.
4. Turret is direct .75x.75 square tool mount. Blade block mounts very solid in turret but is pushed out about .500" from OD of turret. Blade is then extended 1.00" from blade block.
5. I ran end to end on the side of the blade with an indicator and it will change about .003 end to end. Very hard to check up and down

All in all, I am pretty puzzled and ready to test a totally different tool and see what happens. It might also be that the runout issues on the chuck are an issue for this. Sometimes you will clamp and get .002 runout, sometimes .005. TIR that is.

I got some of the worn noise and finish issues when the bar was done and only held in the chuck. I am running three parts per chucking, .600 long, extending bar 3" from face of chuck. Not chatter at ALL with WNMG OD insert tool and I take manly cuts.

[tmcallister74]

Originally Posted by bob1112 I keep hearing people say feed harder. I am running 1000sf and clamping spindle speed to 5000. Feed at .003/rev. I am told to go harder with the feed but.... With all this rubbing, I am concerned about that.

So, at .764 dia you a maxxed out on spindle RPM... So you can make 20,000 SFPM, It doesn't really matter. I always had good luck at .002/rev.