Slotting 1018 Steel

I have done a set (25 each) of 1018 steel blocks. I had to cut a slot (approximately 3/4" x 2" x 1/2" deep) into each. Seems simple but I had one heck of a time keeping a tool together. I could do a few and then would kill the edge of the cutter. I used 2 flute carbide with mist water based coolant. I did various speeds and feeds with not much success in getting any tool life. Feeds from 5-10 ipm and speeds in the 1500 rpm range. What would you do to keep the tools alive? This should not be rocket science...tnx

What machine? How many passes?

Sounds like you're burning up the edge. I would start with a good 1/2" 4-flute endmill AlTiN or TiAlN coated and variable index (will run about $40-60).

If you're doing it on a VMC, I'd cut full depth at 4000 RPM and 50 IPM.

A Bridgeport will need to be babied a lot more.

Bridgeport style CNC. Limited top end rpm. I did various depths, from .2" deep to other experiments. Should have been easier then it was!

The speed is a little low, but whatever, that won't kill a tool.

Feed per tooth, light to moderate.

Not running so fast that coolant is going to blow up your cutter.


2 things come to mind. Your endmills are crap, it happens sometimes with
cheapy carbide endmills, they just won't hold together no matter what.
I had it happen once with good endmills, 3 of the batch of 6 I bought just
essentially blew up instantly, replaced quick, no BS.. Thanx Curtis.

The other thing, a 2 fluter probably has more of an aluminum geometry,
not as beefy, higher reliefs, sharper.

What kind of failure are you seeing? Are you re-cutting chips?

I try not to recut the chips- I tend to use the mister with a fair amount of air to clean them out. The failure is on the tip, rounding it off and then burning it.Possibly cheap cutters- I tend to buy them for McMaster.

lorbiecki said:

I try not to recut the chips- I tend to use the mister with a fair amount of air to clean them out. The failure is on the tip, rounding it off and then burning it.Possibly cheap cutters- I tend to buy them for McMaster.

Click to expand...

As a machinist, there are 2 things that will always kick your ass. Lack of rigidity, and a thrashed machine.
The good thing is that if you learn techniques to deal with these things, and can still make good parts and
hit decent tolerances you are going to be a fricken superstar when you get something that is rigid and square and
accurate.

Bridegeport style. Lets just talk about the rigidity, because that, right now is 90% of your problem, or at
least I'm convinced it is.

So you've got a floppy machine. I've got one too, I haven't used it in 12 years, but I have one, and I've used it, and I've made a lot of money on it.

First thing you need to do is pick your tools, and this is really easy. You can go with corn cobs, but that's old school. What you need is variable flute and/or variable helix endmills. You're floppy, you get chatter, you need to break up those harmonics, and that is what these endmills are specifically designed to do. They are awesome on a brick shithouse of a machine, but where they really truly shine, is on a floppy machine.

You're losing your corners.. Because you have a floppy machine. Corner rads. Simple enough.

Try some of these.

TITAN VI-PRO ENDMILL

or these.

1/2 Variable Flute End Mill with 1.25 LOC MariTool

Both of those guys are members here, and both of them will back up their product. *I'll* back up their products, neither one is going to screw you or sell you crap.

So now we are doing what we can with the tool to limit the harmonics and keep the corners from chipping..

I had a series 10 Acroloc... Is that laughter I hear?... 90% of the machine is pretty solid, its not a
monster, but its all box X,Y, and some of the Z, but it runs a Bridgeport style quill with a tool holder
interface that is just somewhere between pitiful.. disgusting.. and embarrassing.. Floppy doesn't begin to
describe it. Noodle-y would be more appropriate.

EVERY tough cut I made, even with the good endmills, busted a corner off first thing, and sometimes it took
the whole tool with it, or the busted corner wedged and screwed it all up. I would actually take a brand
new endmill out of the package and grind a big chamfer on one corner, and then run it. That really really
really broke up the harmonics and I could pretty much do what I wanted within the limitations of the HP
of the machine. It was pretty amazing.

There are some programming techniques that I've used on a CNC knee mill and the Acroloc that can make the machine
seem more rigid than it is. If your interested, I'll expand on that, I probably will anyways, but right now,
I've got to make some phone calls and feed the pups.

Can't go wrong with what Bobw recommended.

Here is a link to our carbide corncob style roughers..

1/2 TIALN rougher MariTool

Nice thing about this one is that the flute length is nice and short at 5/8. Perfect for your application. These corncob roughers aren't going to make any impressive youtube videos but the are as reliable as you can get. Shit I've seen them slot running backwards and not break. Was on a live tool lathe and motor wiring was reversed.

Here is yet another option...

1/2 Variable 4 Flute End Mill with Chip Breaker .625 LOC .008 Radius MariTool

variable flute ALCRN coated with chipbreakers. In 4140 you can slot at 500 sfpm, profile at 900 sfpm. I use them on H-13 tool steel and we get more parts per cutter while increasing speeds and feeds 20%.

Anyway lots of ways to skin a cat.

I have a really crappy casting to set up, so I'll do something to put that off.

So.. My theory, techniques to make a floppy machine perform better.

The theory. Metal moves, we all know this. Machines are made out of metal, they move,
little light machines move easier, simply because there isn't as much metal. But as we
all know, if you bend metal, its gets harder and harder and harder to bend it the further
it bends. Same with stretching a rubber band. So, the trick with a floppy machine is
to get it to bend in one direction, and then KEEP it there.

The hardest on a floppy machine is slotting, as you are finding out. On a straight slot,
the Z axis isn't under any load, its free to bounce and hop and twist and move all over the
place. My trick was to ALWAYS ramp in a slot, put some force back up into the Z, get it bent
a little and make it more rigid.

Profiling. Narrow and deep. A technique used on bigger machines, but just like the variable
helix/flute geometry, it really can make a small floppy machine behave like a bigger more rigid
machine. If your profile will only allow you to take shallow and full width cuts, go back to the
ramping.

The worst thing with a knee mill or a low HP mill. Once you figure out how to make it work for you,
you have to go beyond simple feeds and speeds. You have to start back figuring for Horse Power. The
good thing at that point is you know the machine has nothing more to give.

lorbiecki said:

I have done a set (25 each) of 1018 steel blocks. I had to cut a slot (approximately 3/4" x 2" x 1/2" deep) into each. Seems simple but I had one heck of a time keeping a tool together. I could do a few and then would kill the edge of the cutter. I used 2 flute carbide with mist water based coolant. I did various speeds and feeds with not much success in getting any tool life. Feeds from 5-10 ipm and speeds in the 1500 rpm range. What would you do to keep the tools alive? This should not be rocket science...tnx

Click to expand...

you dont say what size carbide cutter?
sounds too slow for a 2 flute. you would need much faster rpms. you are in HSS territory speeds.my 1/2" 4 fl carbide mill goes 0.150" deep full slotting at 5ipm. 1600rpm.

I havent ran a knee style mill in probably 2 decades other than a few G jobs on a manual Bridgeport....take this with a grain of salt in addition to what others already posted. Back in tech school they told us to NEVER climb cut....I have done nothing but climb cutting on the machining centers I program....If I was programming a knee style machine, especially one with some slop in it, I suspect I would conventional cut (assuming you are not just running a straight line toolpath). Also would check collet / toolholder condition and rigidity of set up. Are you squeezing the slot closed in the vise???

Would a big diameter saw designed for a horizontal mill provide any advantages besides more teeth in the cut to clear more chips. Also the chips would fall away with gravity. They seem to have been replaced with endmills for almost every job.
I know it is not called a saw but I can not come up with the name now. They are the same as a slitting saw but much wider. In this case 1/2 inch wide
Bill D

Bill D said:

Would a big diameter saw designed for a horizontal mill provide any advantages besides more teeth in the cut to clear more chips. Also the chips would fall away with gravity. They seem to have been replaced with endmills for almost every job.
I know it is not called a saw but I c nnot come up with the name now. They are the same as a slitting saw but much wider. In this case 1/2 inch wide
Bill D

Click to expand...

"Milling cutter"

You need a pretty stout machine to wield a 1/2" milling cutter in steel. Like, a 40-taper horizontal with the milling cutter running on an arbor with an outboard support.

Regards.

Mike

So use a 1/8" wide one and take a few extra passes. I wonder if anyone has ever made an outboard bearing for a bridgeport using a milling cutter horizontally.
Bil lD

Bobw said:

You're losing your corners.. Because you have a floppy machine. Corner rads. Simple enough.

Click to expand...

Didn't know that. Always wondered why the small radius endmills I'd acquired lost their corners instantly on a bridgeport. Maybe it wasn't my fault after all. Always have worked well at side milling though.

Thanks.