Machining 316 3

[bananamga]

I'm having difficulty machining 316 on my CNC Mill. I'm using a 1/4", 4 FL, carbide end mill to cut a cavity out of a bar of 316 stainless, and consistantly chip my tool. (so far, it's chipped every time I've used it) I'm used to machining 303S, which seems like butter comparatively. My spindle rate is 1100 rpms, my linear feed rate fluctuates between 2.0 and 1.5. I hear chatterring when the tool changes direction from the X to Y axis, or vice versa. I've even tried a cobolt cutter, with no success. Does anyone have any suggestions? Perhaps 316 isn't the solution...I picked it for it's corrosion resistance. Is 304 or 304L any easier to machine?

 

[EdStainless]

How much material are you cutting? You need to cut deep, even if it means slowing down. Shallow cut will work harden the surface and make it very difficult to machine.

= = = = = = = = = = = = = = = = = = = =
Corrosion never sleeps, but it can be managed.

http://www.trenttube.com/Trent/tech_form.htm

 

[bananamga]

The cavities are .290" deep. I've been slotting them at .145" increments. Then side milling them at lengths ranging between .535" and .945". Also, my linear feed rate mentioned above is in mm/sec. Thanks for the advise, and any more that may follow.

 

[strokersix]

You may need to slow down and use a high speed cutter instead of carbide, perhaps TiN coated. Also, cutting oil may help instead of water based machining coolant. Confirming what EdStainless says, you need to always pull a reasonably thick chip. If you try to take thin chips the material will work harden and cause trouble. Also, climb milling is better than conventional if possible because each cutting edge will begin on fresh metal taking a thick chip. It may be easier to get thick chips if you take three or four passes to get to .290 depth instead of two although that's a trade-off because the cutter end is doing all the work.

 

[Metalguy]

Bananamga,
304/304L will work-harden faster than 316, so if that's your problem you shouldn't change to them.

 

[BillPSU]

Bananamga,
You are running a 72 sfpm at 1100 RPM which is low for carbide. It perfers the higher speed 2000-2500 rpm. The rigidity of the setup is always a consideration. I would try 2000-2500 rpm at 3-4 mm/s. If it chips, I would recommend switching to HSS cutter with a roughing cutter and a finish cutter. Increase the feed rate on the HSS to 2-3 mm/s.