parting off aluminum

[harpman28]

Hello. The company I work for just bought a brand new Haas sl-20 lathe with all the bells and whistles (bar pusher, live tooling, programmable tailstock etc). I don't have very much experience with cnc lathes but am catching on quickly as I do have much experience on the manual lathes and VMC's. The problem I am having and was looking for some advice on, is parting off aluminum. We purchased a Seco insert cut off blade, the 150.10 hss blade with both general purpose TP25M and HX inserts recommended for aluminum. For steel the the general purpose TP25M with a neutral cutting edge worked very well cutting off to center and leaving only a minimal nip on the back of the part while leaving a beautiful finish. I have tried both the inserts in aluminum and the results are terrible. A cottage cheese like surface with a visible consistant toolpath on top of it. I have played around with the height of the tool, a bit below, right on and a bit above center. I have only as much blade sticking out as I need, which is about .75" and the tool is getting flooded with fresh coolant. I have talked to Seco tech guys and have pushed the tool thru a very wide range of feeds and speeds, 390sfpm .004ipr to 1200sfpm and .012ipr, and the results have been the same everytime. I am not cutting to center and have finish turned the surface where the tool enters the part. So I guess what I am wondering is, now that I have tried the seco, what can you guys recommend? My boss wants a nice finish without a second operation. I am looking into the Empire twin tip cutoff system as I have heard good things about that, but if anybody has any other ideas or recommendations on my current set up I would love the input. Thank you for your time.

Big D

[Delw]

if your not cutting to your center your tool is not on center or your turret is off center.

ooops sorry your talking about the part that is cut off.
use one of the angle cut off inserts, but you will always get a tit on it, nothing you can do about it.
we usually just lap the back of the part on some sand paper if your print allows. that will take the tit right off.
to get a smaller tit on the back try this
the smaller the part the less of a tit.
the smaller the thickness of the cut off the less of the tit
use a sharp corner cut off tool and the tit will be smaller also.
use and angled cut-off tool
slow your feed down to .001 about .100 dia. and the tit will be smaller as well.

[harpman28]

Thanks for the advice. I would love to try the right hand inserts for this blade, but unfortunately they seem hard to come by in the HX grade. I had to submit a special quote through J&L that would take a minimum of 2 days(it has been 4 now) for Seco to tell me when or if I could get them and how much. I find this rediculous as they are listed in their catalog. So anybody with a hot set up for a cutting off aluminum and leaving a nice finish? Do the right hand inserts really leave a much better finish? I would love to jam a hss or carbide tipped P type blade in there like I would on a manual lathe but the majority of holders for these blades are not meant for cnc is seems.

[Delw]

what dia is your part?

[harpman28]

OD is 1.75"
ID is .75"

[Delw]

oh so its a through hole?

thats an easy one for no second op, the tool your using is fine

first grab a threading tool and do a 45 degree angle in the bore to were it will cut-off so you have break in there when the part is parted off. as along as its per print.

just feed .001-.002 at 3000 and above rpms

if you don't get a good finish at that your tool is not set properly or its not parallel

the tool width is what? ( I am to lazy to check)

sure you can go recommended feeds and speed but they are usually wrong for most situations.

if your using a chuck you might have to slow the rpm down slow so the jaws dont ding the part. if your using a collet chuck you will be fine.

[harpman28]

The insert is .122" wide. I just tried it with a .001 and .002 ipr and the same thing occured. A crappy surface finish from OD to ID. I also indicated the blade and it is very straight and so are the parts. They are right on size and flat on the cut off side, just ugly. The chip coming off of it looks like crap too. Curled up but the material is definitely not shearing properly and from the looks of the insert geometry (rake and chipbreaker) it doesn't look like it ever will.

[Delw]

Then your insert is in the tool wrong or your holder is in there wrong, or your part is sticking out way to far from the chuck.


got a digital camera? take a pic of it and post it. take a pic of your set up also and the tool. something isnt right.

thats an extreamly easy part, you shouldn't have any problems at all.
pretty much any grade insert will cut the part off.


just out of curiosity, is your coolant going down the blade or does it only flood? cause if its not going down the blade when the insert is in the part then its not getting coolant.
you can take a piece of copper tubing and route the coolant to the blade if need be. I think you can do that with a has, I know other hitachi, supermax and most others you can.

one other thing you are using an m03 and the tool is facing the correct way.

Delw

[g-codeguy]

What grade of aluminum are you running? We have had an aluminum job set up and running with a beautiful finish. Next bar that loads, and it looks like crap. Nothing we then do seems to help. Load another bar, and it is nice again.

Delw is correct as far as cutting off without leaving a burr. Put a small 45 degree chamfer on the back I.D. Program the tool nose to be tangent to the 45 degree at a point .003 past the c-o point. I have found this to be critical. Usually a neutral insert will work fine, and normally (but not always) cut off with less taper. Chamfer size can be any size, but this .003 dimension has to be held close. I have put as small as .003 x 45 degree break on the c-o end and had the part drop off clean. Use a threading tool with .002R to a maximum .004R for best results.

I would try a PVD coated insert as their edges are normally sharper. At least those from Kennametal are. We cut off washers as thin as .034 using Manchester 507-240 M45 inserts (.094 wide). Even done it with a .062 wide top notch groove tool, tho I do prefer a smaller than .008R on my c-o in most cases. Depends on material being cut.

We have one or more lathes running end washers this way every day. It won't take you long to figure out which direction in Z-axis to move the tool. No burr on the cut-off face, but the burr pushes onto the bore side, then move Z-axis minus. If a little hump on the c-o surface, move Z-axis plus. With a little experience you will be dropping parts off with next to nothing (burrs) on the c-o end.

[djr76]

Does the insert have a chip breaker?, that might help. Its sounds more of a lubrication problem like Delw suspects.

[307startup]

It probably has more to do with your aluminum supply than anything else. Two sticks of 6061-T6 from the same batch will cut very differently because of the minor differences in chemistry.
Are you running constant surface speed as you part off? And have you tried a peck cycle part off?

[neilw20]

To change hands you can put the tool in upside down (if it will fit), and run the spindle in the oposite direction.