[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...
[ame=http://www.youtube.com/watch?v=5fTSqAoZzNE]Parting Off Geometry Demo.wmv - YouTube[/ame]

This is what it shouldn't look like...
[ame=http://www.youtube.com/watch?v=b9tIlCVm12Q&feature=related]Parting off.wmv - YouTube[/ame]

[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]

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.

[fizzissist]

We're all missing something very obvious here......It's something stupid simple. Has to be.

Could you post some pics?
1. Close up of the blade installed in the toolholder, installed in the turret.
2. Close ups of the insert, top, side, front, oblique
3. ... Face (manually, using handwheel) maybe .01" off the bar with the tool, stopping feed in X so that a .01-.02 nub remains... and take a close up so we can see the surface finish on the bar side, and where the tip is relative to the CL (not that we think you're fibbing about the CL.... we just wanna see)

This problem is pissin' me off, and I wanna see you with a happy cutoff.

[jimmyjolly]

Where is the material sourced from? We use a huge amount of 6061 t6 from varying suppliers, we have found certain batches coming in from china to be right on the limit of the t6 temper making it almost impossible to cut, just gums up and even using steel tips and insane feed rates cannot get any chip breakage. I would suggest trying another supplier for your 6061 or failing that, can you get away with using 6262 t6? It anodizes well, has similar shear strength and machines like a breeze!

I would try and bump up the concentration of your coolant mix too, always helps on aluminium, and if you are having trouble with chip breakage, use a more negative steel insert, just steer away from TiN coatings.

Another thing, is the coolant directed onto the tip the whole way through the cut? Probably sounds like a stupid question, but coolant flow is critical for parting, make sure you have a consistent flow the whole way through the cut.

Hope you have some luck!:cheers:

[neilw20]

Try some WD40 or kerosene from a spray bottle.
Your chips are screwing out crooked so tool is not square, or forces are causing misalignment. Chip exit path on top of tool must be smooth.
0.002-0.003 per rev. Front clearance 3-4°. Top rake at least 5-6°. VERY sharp.
If the machine can't take the force and deflects use a narrower tool so the deflection is less because of lighter load.
Chips screwing sideways are damaging the face.

[PixMan]

Walter makes a single-ended insert designed specifically for parting off aluminum. It looks nothing like the CF6, CF5 or CE4 shown in their video that was posted. Nor does it look like any other insert made by any other company. It is the CK8 chpbreaker, available in the FX2.2, FX3.1 and FX4.1 size single-ended inserts and in only the uncoated grade WK1. It fits only in their 26 and 32mm tall "XLCFN" blades (so far as I know.)

I've tried almost every parting tool known to man, from hand-ground HSS tools to various single and double-ended inserts. Nothing else seem to work quite so perfect!

[bob1112]

Sorry guys, been busy with work and kids.. Coolant is at 6% and carefully aimed to supply coolant inside the cut.

Something to consider, I am running the blade as LH and M4. I do believe the holder block is reversable and the insert does come up to CL but something I should add I guess.

I will work on some pics. I have a couple jobs that that need my attention on the mills but I DO want to work this cut off issue out on the lathe. Very much appreciate the help from you guys! I cannot help but think it is something simple that I am missing here. Going to be irritated/happy when I find it!:idea:

[littlerob]

I hate to be that guy that suggests you buy a new tool holder, because I often think to myself "hey I just gotta get through these parts a$$".

But I never use part off blades, unless absolutely necessary. I use groove/turn tool holders, and at that diameter you might want to think about it. You have much more control over what you want to do, even if it still sucks you can leave stock for a finish pass like fizzissist suggested, but I can never get it to work with a part off blade.

Robert

[bob1112]

I was close to abandoning the blade but would have to replace them with multiple single ended holders because I adjust them a lot for the most rigid setup. There seems to be several people using them without issue which is damn frustrating. Been working with mills for years and know feeds/speeds pretty well and just cannot find a spot where the blade works. Even the inserts were confirmed to be specifically ground for Al but I still think the major issue is they are dragging on the sides for some reason. I just don't think another holder will help but I will see if I can find another in the shop to try.

I do have a tool rep coming out on Monday WITH some other "expert". I told the guy if he does not have experience, this is a wasted visit because I have done about everything any machinist would know to try. maybe we can find the issue.

[littlerob]

I do have a tool rep coming out on Monday WITH some other "expert". I told the guy if he does not have experience, this is a wasted visit because I have done about everything any machinist would know to try. maybe we can find the issue.

I love those visits (not), I spent 3 hours with a guy last week whose tool failed again and again. You haven't tried everything, otherwise your parts would be coming out the way wanted, sorry. Even the video that was posted was not a part off blade it was a grooving tool. There is so much deflection with a part off blade, that is why you were getting convex part shapes before.

If you are going to stick with it though, here is some geometry knowledge: the geometry of the insert on a part off tool is designed to make the chip curl up on the flanks, making the chip narrower than the groove itself, allowing coolant in and allowing the chip to get out. The key to making that work is pushing the tool hard enough to generate that chip. I don't care much about SFM when parting, go low it will generate less heat, but feed is important, .005 in AL is no big deal.

But if you can find a groove tool that will do it that is where my next step would be personally.

Robert