Slot milling w/ .0312 endmill

[extanker59]

I'm milling 6 .04 wide slots, equally spaced, on a 5/16 dia part. The slots are about .052 deep. Material is 17-4ph. Not hardened yet.
Roughing with one end mill, finishing with another. Finisher still going, roughers lasting 1.5 parts. Both endmills are 4 flute stubs (tried 2 flute std but it broke right away).
My attempts are 11,000 rpm, 1.5 ipm, .015 doc
11,000, 1.0 ipm, .015 doc
11,000 1.0 ipm .01 doc
9,000, 1.0 ipm, .01 doc
Can somebody help?

edit: sorry. using carbide endmills

[beege]

Might work better as hardened. 17-4 cuts better at H900, H950, etc. You aren't going to get that tool up to the proper speed, so the speed you are going isn't going to matter much. I'd rough slower, though, maybe .7ipm, two or three flute stub.

[extanker59]

Thanks, I'll try slower next part.

[HuFlungDung]

I don't think this stuff comes in "non-hardened" condition , not that I've yet had a project that called for it.

http://www.aksteel.com/pdf/markets_p...Data_Sheet.pdf

Even condition A is Rc35

Anyways, this type of difficult slotting is something that I use OneCNC's high speed toolpath for. I checked to be sure, and yes, it will create a looping toolpath with a .031 diameter tool, down a slot .040 wide with .001 finishing allowance. The advantage is avoiding that full width tool engagment that is so hard on a tiny little tool.

I mention this because many people are not familiar with the concept and think nothing else is possible but full width cutter engagements to open up a slot.

[extanker59]

Lol, ok, ok, I meant it gets even harder later.

Yeah, I've been seeing these tool paths advertised by several cam systems. Unfortunately, I'm stuck doing it the old way. Any suggestions?

[silverfoxx03]

I have machined this successfully with Destiny tools. I was using a 1/2 dia endmill going 1/2 deep with a full engagement at 1000 RPM and 30 IPM.
Walked right thru it and made literally not a bit of noise.

[HuFlungDung]

Originally Posted by extanker59 Lol, ok, ok, I meant it gets even harder later. Yeah, I've been seeing these tool paths advertised by several cam systems. Unfortunately, I'm stuck doing it the old way. Any suggestions?

Drill a plunge point or helix down into it, since you'd have to cope with the conical drill point at the bottom anyways.

Perhaps you can draw your own looping toolpath. If you have cadcam software, you can draw a series of overlapping circles....just enough to make two complete tool circuits in the loops, trim the entities to save just what you need, then copy and paste enough copies end to end to make the length of the slot. Then use some simple cut chain type operation on them.

IIRC, someone on these forums may have written some kind of a macro to do this type of machining on simple shapes.

[Delw]

I dont know what type of endmills your using but dont go more than a .025 pass with a endmill that small. I am guessing .015 tops.
a stub endmill will help big time and you may be able to go deeper.

No offence to huflungdung, but dont drill a spot hole you will break more endmills on small slots like that. the burrs get in the way and grab the tool into the part

I dont know your situation as sometimes you have to use a endmill, but personally I would be using a slitting saw not an endmil. even if it requires a second op the slitting saw is the only way to go.

also dont forget the smaller the endmill dia. the better the tool run out must be, you can get by but you have to cut your speeds in half if you have too much runout.

[HuFlungDung]

Oops, no offence taken, but I could have specified to drill a plunge point with a spot drill A ramp into the cut would be better except that it is still a full width entry.

[Geof]

Originally Posted by extanker59 Lol, ok, ok, I meant it gets even harder later. Yeah, I've been seeing these tool paths advertised by several cam systems. Unfortunately, I'm stuck doing it the old way. Any suggestions?

Is it a straight slot?

Do it the old fashioned way, something like 30 lines of code and about 30 minutes to write it.

Have a look here: http://www.cnczone.com/forums/showth...t=73902&page=4

Posts 67, 73 and 74, code is in Post 73 all you need to do is delete the multiple subroutine calls, change a few coordinates and feeds.

[Delw]

Understood, I guess I could have read it better too.

I had the same part almost funny, cause it was the same dia ( had a thru-hole) same slot size. depth I think was like .060 -.001 +.000. .304ss 303ss and 17-4 ph
I ran hundreds of them, most boring job in the world and the slowest by far.
I had a cam system so I just programmed a non stop loop for the slots speed it up on the no cutting parts slowed it down on the cutting parts in the program.

anyhow. I tried everything including drilling a ton of holes in the slots to take out the material and what I found was that the burr edge would suck into the cutter and snap me off.

even put them on a 4th axis to rough the slots, then turn it up to finish didnt work either cause the rad. when the 4th was at a ninety causes burrs and snapped me off when the 4th was upright.

the 303 wasnt that much easier like I thought it would be.

[Delw]

heres a pic of another one this one I believe was either 15-5 or 17-4 could be 303( dont have my glass's on) I ran it in 1999,
just happened to be doing some cleaning over the weekend and saw about 60 scrapped ones in a box and tossed them.

they are scrap cause they needed a .003 max rad on every side and the operator wasn't paying attention to the O.D. dia. it was easier to scrap them then debur them.

Delw