VMC work. 15-5 H1025 deep cuts + finish

[AgentStone]

So I was wondering what those experienced roughing and finishing (with a nice finish) would use to cut a part out of a 3"x4"x6" block of 15-5 H1025.

I have some experience with the stuff and think I would lean towards a 5 flute endmill or so (helical maybe) and do some chip thinning. It's about 40 rockwell.

I have some tall vertical features to finish. Walls etc... that are 3.25 inches tall.. My main questions are would it be a good idea to try and finish that all at once with a long flute endmill.... OR.. maybe get a solid shank endmill with only 1.0"LOC and step it down.....

Anyways... just curious what those with time in the realm of heat treated 15-5SS would use... as far as tooling and approach...

Thank you for any input!

P.S.. What about reaming a small hole.. (.1242"-1246") reamer brands? SnF?

 

[Milland]

Carbide reamer and drill for the small hole (I like MA Ford). 3/4" or whatever you can fit cobalt stub drill to make entry holes to near-full depth for a 1/2" endmill for the main cavity cleaning. Use whatever you like for the EM but be sure to have positive chip removal either with good coolant flow or mist.

"get a solid shank endmill with only 1.0"LOC and step it down" - This.

 

[AgentStone]

Milland,

What exactly do you mean by positive chip removal? Any particular endmill you would lean towards? As far as flute count and cutting speed?

 

[Milland]

As in, when you have deep features it's tough to get all the chips out, but recutting hard SS chips is death to carbide endmills. So you want well-aimed coolant nozzles or mist blasters to aggressively flush/blow chips from the pockets.

Don't let the cobalt stub drill (or carbide insert drill if that's the way you go) get dull, have spares to swap out to keep a sharp edge.

I'd look for a quality carbide four-flute necked endmill, maybe AlTin coated or whatever's hot today with a vari-flute grind and plan on replacing them at some interval. Flute count and other stuff is something I can't go further with without running your machine and knowing what it likes (stays out of harmonics zones).

 

[AgentStone]

Well... I just wanted to update for those who may want to know about tooling and SnF in the future for this material with some real shop trials.

I've been having great success with using more "budget" like 1/2" endmills for the shorter lengths(.625"-1.25"). Using GARR VRX Series endmills. 4 fluters at around 250-300SFM. 15% radial stepover at around .0028IPT Chipload (~26IPM Feed)

For the long guy in the deep pockets, Im using a HELICAL#82902 Ø.500" 5FL (*Chipbreaker*) Bullmill R.030 .625LOC with 3.375" of reach. Utilizing about .500" axial depth cuts, 172 SFM (1320RPM), with 10% radial stepover (.050") and a feed of 13 IPM (.002" chipload)... Let me tell you... This 5-flute dream is whispering through that hardened 15-5.. Im blown away... then again... there's nothing like the right tool for the job... I just hate cutting tough steels like that with anything less than 5-flute... However the 4s did do ok in the shorter lengths... I would have much preferred 5 for all but you know.... cheap boss...

P.S.

Check out the look of the chips of `15-5 (40HRC) from that long (3.375" Reach) 5 flute Helical endmill. **Attached below