Stainless steel 15-5P

[cncfrank]

Hey All: I'm new to cutting Stainless, and I now have a job to cut 15-5P, I have looked it up, and can't find that stainless available as a material in the Mastercam Library. Does anyone know of a similair material that is in the library.....like 304.

 

Thanks,

Frank

[Mr. M]

17-4 maybe??

[cncfrank]

17-4 isn't in the Mastercam Library either ?

[chris m]

17-4 is pretty close. 15-5 and 17-4 annealed cut like sh!t, very tough and gummy. The harder stuff cuts better [H1075 H1100 H1150] from a chip removal standpoint but SFM remains pretty low. If you are turning I'd expect to be in the 400 SFM range for carbide and maybe 500 with a cermet insert. I'd suggest moderate depths of cut with a pretty aggressive feed [50% of TNR] to help break the damned chips. If you are milling I suggest using inserted tools with the proper inserts or purpose-made solid carbide [Z-Carb, Varimill, whatever] in order to get any decent tool life; milling or drilling with a vanilla brite carbide tool is going to make for a long day.

[cncfrank]

Thanks Chris, I've allready been told to order Z-carbs for the cutting, I just thought Mastercam would have it as a material pick in it's library. I guess I can just get a starting point feedrate...in the Z-carb cat. Sorry I'm milling with X2 MR2 SP1.

[Mr. M]

A+ chris

[strabe]

Use 304 from the material library if your material is in the annealed condition. Use 303 if it's in H1075 or H1100. As Chris stated it machines so much nicer when it's been heat treated just like 303, but just like 304 if it's annealed.

 

Good luck.

[Thee Dragracer1951]

It's nastier than 304 if it's annealed....

I do some parts for a marine assembly every month. I keep on tellin the customer to heat treat the material. he never does. I cut it up and put it in the HT furnace in the corner...

I learned that one after I trashed about $200 worth og threaders one day before I realized the stuff was annealed.....

[gwilliams]

We cut a lot of parts out of 15-5P, heat treated and annealed. I’ve found light radial cuts (.060") work the best for a compromise of tool life and speed. I would typically run around 450SFM with a chip load of about .009" per flute (the .009" actually calcs out to aprox .005 per flute using chip thinning). I would also recommend using as much of the flute length as possible in the cut. The one major thing to watch for is that the tool does run into any corners where the tool would be engaged more than 30% or so.

 

Good luck