[Talisman]

Anyone have any experience with this stuff? I'm told its 36-40 rockwell. I have to mill 48 .260 wide slots about an inch and a half long in this stuff. The stock is .225 thick. I'll definitely be using carbide mills and drills for pilot holes... Any help with feeds speeds, doc, chipload, sfpm etc... This will be done on a haas VF3, 7500 rpm max spindle speed. I figure i'll start about 130 sfpm maybe .100 DOC? (nuts).

[sportbikeryder]

I have been using Niagara Stabilizer tools on Ti-6-4 and Viscount 44 on a VF5 40T with the same spindle. Depending on how good you need the surface finish, and how good you can hold the part you should be able to get some pretty good material removal rates.

For a 1/4" diameter, they list 350 sfpm and .0009 ipt chipload . They claim 1D slot cutting depth. I have been using very close the listed speeds and feeds at .7D slot depth.

If you can clamp your part to a consumable base plate (aluminum plate), I would get a .250" niagara stabilizer, run it at 5348RPM 18.2 ipm and .13 depth of cut (.13 first pass in material, .095 second pass for breakout)

John

http://http://www.niagaracutter.com/...stabilizer.pdf

[The White Fox]

sportbikeryder made a good call with Niagara, and another good e-mill for this stuff is Iscar and OSG as well as CID tools. I don't think you'll need carbide drills for this stuff (especially @ .225 thick with a .250 clearance hole), unless you're running production, cobalt drills should be fine at about 25 sfm and a 1/4 drill about .005 inch chip load - so I'd run F1.5 - 2.0 @ 375 RPM. Also, if you are running a "stubby" end mill (regular l.o.c. may be fine) you can take a doc = diameter, just drop your rpm's about 20%.

[The White Fox]

Oh yeah, use split point drills, as they tend to have a flatter drill point angle - broad angle for hard stuff and a sharper angle (and chissel point) for soft stuff. Another thing, if you make a huge spot for your drill or have a pilot hole, use a chisel point and/or sharper angle drill point to prevent the hole being over sized near entrance (centering it self as the outer cutting edges hit before the drill point bites in).

[Talisman]

Thanks for the help guys! Also, this isn't a repeat job... its more off an asskissing job making some custom parts for a purchasing guy's chopper .