PDA

View Full Version : End Mill Wear



pntrbl
06-22-2010, 02:37 AM
I'm here hat in hand once again because I seem to be using up endmills at an alarming rate. A new one cuts sweet ..... but not for long!

The machine is a Seig X3 from Harbor Freight with a Noga mister on it. The mister seems to be doing an excellent job in that I can grab the end of the endmill right after shutting it down from a cut. It ain't the slightest bit hot. I'm not burning them down.

The endmills I'm using are from McMaster. Niagara even. Typically 4 flute center cutting because that seems like it'd be more useful for more things. 100 sfpm because I'm typically cutting HRS. I'd run a 1/2" mill in the 800 rpm neighborhood for instance. All feed is manual and it's sure easy to tell when a dull mill starts twisting the X3 up.

I conventional cut whenever possible but occassionally find myself having to climb the other side of something. Almost never plunge.

The specific part of the mills that is getting worn is the corners. To get to my required depth I'll drop the head whatever I think she'll take and with the worn out 1/2" mill that's in there now I can't cut .005 accurately. When it's new and sharp I can get a full width accurate cut at .020 without too much drama.

My current project involves 5" long slots that are 1" wide. Depth varies from a 2" long section that's 1" deep, connected to an 8 degree angled section that runs over the 3 remaining inches. Comes out a 9/16" deep on the other end.

What I'm not doing is attempting to take out all that steel with an endmill! Running a pair of .450 drilled holes in from the ends at the right angles followed by a band saw cut gets 75% of the material removed before I ever take an endmill to it. Even at that tho I swear I'll need a new mill for each piece. This could get expensive .....

I think I'm gonna try some roughers and save my 4 fluters for the last .020 or so, but if I'm doing something really stupid here I'd sure like to know!

SP

Blackadder
06-22-2010, 03:38 AM
800 rpm is a wee bit fast

HRS sfm =80 or so


so 80 * 4 / (end mill size) 0.5 = 640 rpm


for a X3 style mill drop it down to 500 rpm



maybe that why you are using cutters up

Stuart

beanbag
06-22-2010, 04:18 AM
conventional cut also tends to wear out endmills, but your machine isn't stiff enough to climb cut.

What's your approximate feed rate?

oldtiffie
06-22-2010, 08:03 AM
conventional cut also tends to wear out endmills, but your machine isn't stiff enough to climb cut.

What's your approximate feed rate?

Oh I dunno.

http://www.cnckits.com.au/videos_promica.php

BobWarfield
06-22-2010, 08:36 AM
Something else wrong here. 100 SFM is not too fast, though 80 would be more conservative. Still, I run mine at 100 and they seem to last a long long time.

Without knowing more, I would wonder about two things.

First, recutting chips is death on cutters. You're using mist, but how effectively are the chips actually being cleared? Slots are the worst for this. Perhaps a stronger air blast would help.

Second, since it is hot-rolled, I am wondering if there is any possibility there is a little scale? Sometimes there is some hardened material here and there with hot rolled. That too will be a bit harsh on the cutters.

If those aren't issues, try slowing down by all means. Excessive runout on the spindle, vibration, or chatter can also wear the cutter faster.

Cheers,

BW

J Tiers
06-22-2010, 09:26 AM
If it were a drill, and corners were worn/chipped, we would diagnose excess speed. No particularly good reason why that shouldn't be true of end mills also. Corner wear is usually speed.


Could also be that feed is wrong, maybe too slow, so that you spend a lot of time 'rubbing' instead of cutting. "Cutting" doesn't dull a cutter fast, "rubbing" does.

Insufficient feed can act just like too much speed.... they are really the same thing, only speed is worse. BOTH result in minimal depth of cut per tooth, and a lot of "rubbing". It's just that higher speed makes more heat.

if you run a good speed, but feed too little, you rub just as much, but heat less. Still can dull the cutter.

Re-cutting chips is a fact of life, and mist coolant does nothing about that, except to stick the chips onto everything and absolutely guarantee that you will re-cut them. IMO you'd often be better off with more air and less/no coolant.

But that does not usually cause corner wear. It can cause the edges to chip out all over, but usually not just the corners.

Climb cutting has problems with any machine not made to do it. The usual problem is looseness of the feed screws, so that the force inherent in a climb cut 'sucks in" the material, pulling the table in towards the cutter, so the cutter "climbs" onto the work instead of cutting. Even a small mill can do it.

I wouldn't try climb cutting with a small mill, you may break things unless you dust off just a whisper of material. And even then, one higher spot and you may 'suck in" the work and have a worse finish than conventional cutting.

Carld
06-22-2010, 10:50 AM
If I understand it correctly your taking a .020" DOC with each pass. If so then I can understand why the corners of the cutter are wearing out. You really need to take at least .100" DOC and that would eliminate 4 of the passes your now making.

Having looked at a photo of your mill on a site I think your going have to buy a bigger machine to do what you want. Never use a boy to do a mans job.

MTNGUN
06-22-2010, 11:16 AM
Never run an X3, but have a 6x benchtop mill, which may be in the same class, rigidity-wise.

I use roughers for all but the final pass. Much, much easier on the machine, and the roughers seem to hold up better than regular end mills.

1/2" would be a pretty big cut for my 6x. I've done it, but it's much happier with a 1/4" rougher. When the machine starts flexing in the cut, that can shorten tool life dramatically.

I went through a lot of expensive end mills before I learned my machine's limitations. The benchtop mills are capable of doing real production work, but ya gotta play by their rules.

Forrest Addy
06-22-2010, 11:33 AM
Hm. What are your expectation for cutter life? An endmill (any cutting edge for that matter) can be expected to lasts 1 to 3 hours actual cutting time.

You say your cutting HRS as in hot tooled steel? Adherant mill scale on HR steel is very abrasive. If you have a way to remove it (wire brushing, pickling, or a scrub with a disk sander) your cutter life will double or triple depending on how much of your cut time is spent peneteraton scale.

Are you brushing away or picking up the chips as you make them? re-cuttng chips is tough on cutters too. I have a shop vac right at the milling machine. It's sole job is to pick up mill chips. It makes point of operation cleanliness a mere suck away.

Black_Moons
06-22-2010, 01:44 PM
Hmm, Id take a good look at those endmills. How sharp is the corner?
an endmill with a sharp corner will wear out the corner fast, this is why endmills are rarely 'sharp' on the corner but actualy have a radius, though sometimes its a tiny radius.

a rougher is allways a great idea/addition to the toolkit, they make nice SMALL chips that vacuum up a little easyer.. :)

Scale will indeed wear the hell outta your endmill fast. DOC isent bad but is a little shallow.

4 flute is *bad* for slots! Use 2 or 3 flute but never 4

with a 4 flute, the flute cutting out front will push one side flute into the work, bending the endmill with ease, a 2 or 3 flute cutter is more 'balanced' while cutting. Also, 4 flute leaves little room for chips to go and makes sucking chips out harder. Save your 4 flute for the finishing pass once the hole is allready bigger then the endmill so only one side of the endmill is cutting.

100SFM should be fine. Maybe 80 might be a little better.. But should'nt make that big a diffrence.

pntrbl
06-22-2010, 10:18 PM
Thanx for all the thoughts guys and I'll plead guilt through ignorance on most of 'em .....

1/4" rougher coming up.

SP