feeds and rpm's???

[buck30]

i got this urgent weekend job going here.Machining a helical groove around a .15 dia heat treated 416 ss about 50 RC.

tyhe notes i have on the job put the feed at 2 ipm and 4500 rpm but my robob drill had got heaps more rpm's than that and i would love to be not here all weekend.

oh the groove is .015 deep finished and am using a carbide .015 end mill and my max. RPM is 25000

 

obviously the problem is breaking endmills, fixturing is pretty "tight" so vibration is minimal

[Colin Gilchrist]

25000 RPM, 8-12 IPM, depending on what the endmill will take...

 

1% of your diameter is .00015, so I would start with that value for you FPT. That would put you at 15 IPM (.0006 per rev). That sounds maybe a little fast though, which is why I suggested 8-12.

 

Regardless of the feed you end up at, you should be turning 25k rpm.

 

At 25,000 RPM, you are only at around 100 SFM.

 

When I calculated out the ideal RPM, it was over 100K...

[jhjr]

That sounds pretty conservative. 50 is hard but your specs sound slow. 4500 comes out to about 18sfm. Iscar recommends 100-130 sfm for 55 hrc which = 25,000 to 33,000 rpm. Hth.

[Chris Rizzo]

Sounds like a good application for some dynamic milling. I don't think there is anyone with data for cutters that small yet, but a fair amount of ss at least. This may give your some ideas still.

 

dynamic mill feed/speed database

 

If you end up with some pretty impressive results it would be much appreciated by all to share them. Here is the upload form.

 

dyanamic mill data collet form

 

If you need any help with any of the other parameters of the dynamic toolpaths I'd be happy to help.

[buck30]

what sort of depth would you be taking???? been trying 25000 at between 8-12 ipm and .005 depth od cut but breaks the end mill after about 5 minutes work. gopt a little .015 end mill graveyard going here. now cutting it back to .002 deep and see what happens

[jhjr]

I'd think even at .0025 you'd still get the job done much quicker with the increased feed. With that small of an endmill .005, 33% of dia would be heavy if your cutting full width. 10-20% sounds more in the ballpark. Side cutting would be ok at .005 or heavier.