Milling Brass 360, recommendations?

[skyline]

Just as the title states, I'd like to get some recommendations on milling/drilling and reaming Brass 360. Cutter selection, machine parameters, tool geometry and such. Thanks.

[djr76]

Its free machining stuff, go fast with it with carbide if possible. You can always call your tooling guys and they should give you tech support.

175 sfm drilling and reaming with hss

250-350 sfm milling with hss

800-1500 sfm milling with carbide

.004 - .008 chip load

2 -3 flute cutters will work good

[skyline]

Would high helix angle tools work well with this material (milling), also what angle would work well in terms of drilling?

[fuzzyracing1967]

Never tried any milling of brass with high helix,but have done wide veriety of milling in brass and can tell you it will take most anything you throw at it.We have jobs where were taking slow heavy cuts with 1.25 three flute hss,to a job that was just run the other day where it's more of a high speed maching kind of thing,.5625 indexable mill feeding at 50 to 100 ipm. taking .025 cuts.So it's pretty forgiving,as far as the drilling there realy ain't a differance there eather,but if there through holes a little trick is to dull the lead edge so the brass dosn't grab the drill and want to pull it through.

[skyline]

fuzzyracing... thanks for the tip on dulling the leading edge, I'll remember that one.

This material is very forgiving and I love the way that it cuts. We got the brass from a specialty source in brass&Cu so we were sure it's 360. They do metrology on it to verify that it's really Brass 360, and I also like the fact that it doesn't oxidize as quickly. I just diamond turned a plate to optical finish with it. I haven't characterized it yet, but I'm estimating it to be around 10nm RMS..

I'll let you guys know what I get when I characterize it on the white light interferometer (WYKO).

One lesson I did learn on this project was to never use left spiral flutes/right hand cut reamers, on blind holes.. "duh" I believe it's designed to push swarf foward so in a blind hole that's not good. =-)

[Geof]

Originally Posted by skyline Would high helix angle tools work well with this material (milling), also what angle would work well in terms of drilling?

Normally for brass zero top rake is preferred...but this is pretty well impossible with milling cutters and drills. For milling cutters just go with standard helix, for drills just go with standar drills and make sure the work piece is well clamped. On manual machines with backlash and all that stuff it is likely that both mills and drills can pull into the part because they do have an effective top rake. On CNC when everything is backlash free this is not a problem.

Coolant is not normally needed on brass but one thing it does it keep the fine chips from getting into everything.

And a comment on 'dulling' the leading edge of as drill; to me dulling means rounding off the cutting edge and in my experience that is not what you want. Grind a small flat on the cutting edge so it makes a sharp right angle with the tip; this gives your cutting edge zero top rake but it is still sharp.

[Lew Hartswick]

Originally Posted by Geof And a comment on 'dulling' the leading edge of as drill; to me dulling means rounding off the cutting edge and in my experience that is not what you want. Grind a small flat on the cutting edge so it makes a sharp right angle with the tip; this gives your cutting edge zero top rake but it is still sharp.

That always irratates me too. If it's "dull" it dosent cut. That isn't the same thing
as "zero" rake. It should still be "SHARP" . :-(
...lew...

[skyline]

Thanks guys for the tip. Actually one of my co-workers recommended the same thing. Cutting a flat on the leading edge.... he says that it works well on plastics as well when popping a through hole.

I've tried a 45 degree high helix 2fl carbide em and it cuts pretty well and fast. However, when finish machining in lower feeds it tends to produce burring issues..

So back to standard mills for finishing.

[fuzzyracing1967]

Lew Hartswick,Geof

Yes you guys are right,it is not dulling the edge but after saying it that way for all these years and then showing others how to do it,me mouth and fingers work the same.

[Geof]

Originally Posted by skyline Thanks guys for the tip. Actually one of my co-workers recommended the same thing. Cutting a flat on the leading edge.... he says that it works well on plastics as well when popping a through hole....

On acrylic, (Plexiglas, Perspex) and Delrin, yes.

On polcarbonate (Lexan, Tuffak) and ABS, no.

[fuzzyracing1967]

On acrylic, (Plexiglas, Perspex) and Delrin, yes.

On polcarbonate (Lexan, Tuffak) and ABS, no.


Ok,now you got me wondering,why? I never cut any of those,so that's why I ask,the only thing nonmatalic that I'v done was teflon,(I would guess that's in the acrlic family)?

[Geof]

Originally Posted by fuzzyracing1967 On acrylic, (Plexiglas, Perspex) and Delrin, yes. On polcarbonate (Lexan, Tuffak) and ABS, no. Ok,now you got me wondering,why? I never cut any of those,so that's why I ask,the only thing nonmatalic that I'v done was teflon,(I would guess that's in the acrlic family)?

No, teflon is in the teflon family...I am not being a smart-ass, Teflon is quite a distinct plastic very different to nearly all other plastics. Acrylic, Delrin Polycarbonate, ABS, Polyester, Polyethylene, Polyurethane, Nylon all contain Carbon, Hydrogen, Oxygen and for Polyurethane and Nylon also Nitrogen; Teflon is Carbon and Fluorine.

For machining Teflon you need a very sharp edge and a large top rake. You need to kinda slice the material off. Polyethylene is similar, that is HDPE or UHMW polyethylene, it is best to have a tool that tends to slice it.