[trademark]

I may (or may not) quote a job that has a .062 wide slot in 304 ss.
Slot is .25 deep . But it is close to another feature so I would have to use a
.45 long endmill. Slot is .18 long.
I figure i will drill 3 holes slightly smaller than .062 and mill the waste in between.

can any one give me some tips on doing this.
Is there any special cutters that will help with this job?

Or should i walk away ( or run ) from this one

[txcncman]

Just price it so high that if you do get the job, there is enough profit to send the parts for EDM. Let the customer say no. Brokering parts for the right price can still make you money.

[fizzissist]

If you do mill it, use a 3fl from Dataflute. Don't go more than 1/2xdia deep/pass, make sure you're clearing chips. It'll work.

In the alternative, you could use an EDM sinker. Not as fast, but xlnt quality.
As txcncman points out... there are times when it's better to sub it out and give yourself a piece of the action. Just like a general contractor building a house does.

[BobWarfield]

Deflection is going to be a killer on that deep a slot with that tiny cutter. I'm not sure based on the numbers I see that even fizzissist's strategy will work with EM's this small and that much stickout.

Gonna be a hairy job that'll take a lot of light passes to make it work. The numbers from G-Wizard suggest no more than 0.002" deeper each pass. EDM might be faster at that rate.

It might also be worth a tool change. If you run one EM with 0.2" stickout it can go 1/3 diameter deep passes down to 0.2'ish depth. Then switch to one with more stickout and make shallower passes.

Best,

BW

[ihavenofish]

I may (or may not) quote a job that has a .062 wide slot in 304 ss.
Slot is .25 deep . But it is close to another feature so I would have to use a
.45 long endmill. Slot is .18 long.
I figure i will drill 3 holes slightly smaller than .062 and mill the waste in between.

can any one give me some tips on doing this.
Is there any special cutters that will help with this job?

Or should i walk away ( or run ) from this one

304ss.... RUN!

but, if you dont want to run:

1/16" 4 flute tialn ball nose, .01" passes ramping down all the way never plunge. 5000rpm, 0.0005" feed per tooth (10ipm). DROWN the thing under coolant (make a dam if need be).

the method to the madness here is that ramping in with a ball nose will prevent the bit from buckling, lessening the likelyhood of it snapping as the tools gets deeper, or widening the slot beyond spec.

the speed and feed is one if had actual luck with before. the shallow depth makes the chips more of a powder.. which you can flush out as you go. they wont clog the bit. you may want to go even shallower due to the length of the bit. the feed rate is agressive, which helps prevent work hardening. the one thing ive learned about 304, is that you want to take the heaviest bite the tool and machine will allow.

but seriosuly... RUN!

[fizzissist]

What a bunch of whimps.

Drilling the holes to remove the bulk of the material works well, with one caveat... you'll still need to increment your depth cuts, because the little widgets of material left will make the endmill unhappy (I don't know how else to describe it). It'll sound really, really nasty, partly because you're climbing on one side and conventional on the other with very asymmetrical loading on the tool.

I highly recommend against using a ball mill for this, unless it's required.

If you're drilling to near net depth, there's still that bottom to deal with, so you'll need to ramp into it, and I recommend about a 3deg angle of entry. No more.

Whatever you do, do NOT dam it... you need to get those chips OUT OF THERE. Re-cutting chips on a tool that small, at 4xdia depth... not good. The good news is that you can run a healthy air blast on a carbide tool in 304 all day long. You may need to make a nozzle that gets down into the slot for this one.

This is doable... not fun, but doable.

[ihavenofish]

drilling 304 with tiny bits it more scary then milling. may little bits lodged inside the work piece.

the air blast on slotting with a 1/16" cutter, 0.15" deep ive tried, just doesnt work well, eventually the bit snaps as it overheats.

the stuff i mentioned works cause ive done it. of course, im convinced 304 hates me. other stainless grades ive tried have been much more cooperative

if this is a production run, he should try a few different ways and see whats the best balance on time and tool life etc.

[fizzissist]

What kind of cutter...speeds, feeds, DOC, etc??

Drilling a 1/16 hole 4x dia shouldn't be that bad. You need to peck, and don't let it dwell at all, and keep the chips cleared. Use a 135deg split point, new, with a properly spotted hole to start. For this, HSS is fine.

[Shane1234]

im with the ramping program on this one, with a smaller diameter endmill than the slot, ramp & contour. 8000rpm or better, 30ipm, ramp down .002 to .004 per pass, flood coolant. your chips will look like tiny tiny flakes but your ipm's will help you from rubbing off your corners. light and fast will get this done.
I did one yesterday that was similar. I use OSG carbide 4 flute with TIALN coating.