[KVD]

Has anyone done anything similar to this. I've got a 1" inserted helical rougher. And I'm looking to cut 1/2 316 stainless plate. Trough half my cut I will be using the full width of my cutter. This is the most aggresive by far I've ever needed to cut. Can it be done?

[Shane1234]

ive done it in 304, but i do light cuts, .05 deep usually, so either ramping down in helical with my depth set on .05 (not default of angle percent), or depth cuts. the only tool i know that likes full radial cuts is the fine tooth roughers. I get less chatter with a full radial cut than i do with heavy side cutting.

[KVD]

Light cuts would be my choice but boss man wants one pass and it's got my curiosity peaked now.


I'm thinking of putting a .250 Z move in every g1 g2 g3 line to spread the load to most of the cutter and help clear chips while the full dia is involved. Think sawing action. I'm gonna get in touch with kyocera later and get their recomendations on feeds/speeds, but if anyone has exp. close to this I'll appreciate all help.

[rock4xfab]

I just ran 22 parts .625 thick... I started with square blanks. I tried to ramp in and take light cuts and every pass drop in deeper... The cutters did not like that and it was taking way to long.. I ended up .05 a pass full full depth 2600 rpm 18im. The cutter lasted longer ans I actually cut time off the job. I was using .5" v4 4 Flute helical carbide cutters. What took the longest was getting the Profiles down.. Allot of material removal. I should have had the blanks profile lasered and then just did a couple finish pass (this is what I usually do) but the laser was tied up.

[ad64075]

Any indexable tooling would have difficulty with this operation, not to mention that would be pushing the limits on cat40 rigidity, if that's what you are using. Personally, I would use a variable flute solid carbide end mill. Gorilla makes an exceptional tool for this application at a fair price, as well as Garr. Iscar's VFM line is fantastic, however their tool shanks are relieved up to 5x diameter and have a 45' corner, neither of which will help your application.

[KVD]

Smoked the inserts in about 8 sec this afternoon. I'm gonna try it multiple passes tomorrow. Im thinking solid carbide might be better.

[dingo0722]

I've been cutting 5/16" Thick 304 with a 3/8 Cobalt rougher at 710 RPM, 2.5ipm in 2 passes with great success. I tried cutting in a single pass but the tool failed with in 1 inch. I guess the MRR was too high for the tool

[Shane1234]

Smoked the inserts in about 8 sec this afternoon. I'm gonna try it multiple passes tomorrow. Im thinking solid carbide might be better.

if you start to notice chatter, switch to hss or cobalt. solid carbide doesnt like chatter in my experiences.

[dingo0722]

if you start to notice chatter, switch to hss or cobalt. solid carbide doesnt like chatter in my experiences.

I second that. I tried running the same operation with a carbide and found the tool was only able to complete 2 parts before failing on the third. The cobalt is capable of cutting out 22 parts before I switch it out. I have found tool failure in SS is a major pain becasue it work hardens the metal and the material is impossible to cut through at the location of tool failure lowering my yield.

[jamesu229]

.5 slotting cut should be no problem in stainless. 4 flute variable helix, full depth, 150/200 sfm .012 per rev minimum feed. Watch this testing video,feed was .02 per rev, it may help. The main thing is to feed heavy enough to make a thick chip that will be bumped out of the way, rather than a thin one that can be pulled into the cut.

[nomedia="http://www.youtube.com/watch?v=rNF0tp7-vYU"]YouTube- ‪Destructive testing‬‎[/nomedia]

James Urban