[EvolveES]

Hello everyone, i finally had to tackle 304 stainless again. This is pretty much the first time machining #304 (with the exception of the second part i tried on the Tormach and immediately trashed about $100 of end mills and gave up). After this run i no longer fear the dreaded 304.

Images of the parts are shown below with a sharpie for scale. I thought i would share my experiences and results in case it helps anyone else.

I used QUALITY 4 flute carbide end mills, and cobalt 135° split point drill bits (cleveland brand). After making these parts all tools were still sharp and can be used to make more. I didn't break or dull a single tool.

ALL tools were run with the belts in the lower gears for the extra torque in the low RPM
ALL milling was climb milling

"surfacing" was done with a Fullerton 3/8" diameter 4 flute TiAlN coated with a 0.06" corner radius (dont know the PN it was a re-grind off ebay)
spindle speed: 1950rpm, Feed 4ipm, 0.025 DOC @ 0.25 max WOC (.25 stepover).
This recipe also worked for 0.05 DOC @ 0.188 WOC

Milling was done with a Niagra 1/4" diameter 4 flute TiAlN coated, sharp corner (PN EDP N89877)
spindle speed: 1950rpm, Feed 2.3ipm, 0.035 DOC @ full slot and 0.2 WOC

Drilling with a Cleveland LTR I (0.272) 135° Split Point Cobalt Screw Length Drill
spindle speed: 700 RPM, Feed 1.5ipm, 0.19 depth, NO PECK, NO SPOT DRILL

Drilling with a Cleveland #33 (0.113) 135° Split Point Cobalt Screw Length Drill
spindle speed: 1705, Feed: 1.85ipm, 0.19 depth, NO PECK, NO SPOT DRILL

I am sure these are very conservative and could be sped up but they were no hard on tools and got the job done well. The main thing i looked at was the SFM and IPT for the cutters. I kept the drilling SFM right around 50, and the FPT at around 0.0005 for smaller drills, and 0.001 for the LTR I drill. facing SFM was around 190, and the IPT was 0.0005 again. for milling with the 1/4" end mill the SFM was 130 and the IPT was 0.0003 to 0.0004. All of this gave clean shiny chips that were not discolored from heat. I also used flood coolant with Kool Mist 77 mixed a little on the heavy side.

In the end the best advice is to accept that 304 wants to be run painfully slow, and just use the sharpest cutters you can find and focus more on SFM and IPT values than feed and speed values, just tune them to give the SFM and IPT you are looking for.

Hopefully this is helpful and should show good results can be had with 304 in a tormach. After these i am not scared of 304 anymore, i look at it as more of a fun challenge

Attachment 277166Attachment 277168Attachment 277170

[pickled]

Congrats man I am proud of you! Stainless steel is milled every day so there is no reason that we can't do a good job as well. FYI- whatever you do now don't go taunting those stainless steel chips laying around because they might bite at you when you are not looking .

You are going to get a lot of holes out of those drill bits. Those were an excellent choice for the material. Now you need to get some 316L and 440 under your belt before you go and try some real fun stuff like Inconel 625.

[Hirudin]

Are you suggesting against spotting and/or pecking?

To ask a different way, I mean: did you emphasize that you didn't spot or peck to point out how good the drills are, or to point out that spotting and pecking might actually cause problems (like work-hardening or something)?

[popspipes]

Low rpm, sharp tools, positive feed. Some tap magic or something similar helps too.

[EvolveES]

Are you suggesting against spotting and/or pecking?

To ask a different way, I mean: did you emphasize that you didn't spot or peck to point out how good the drills are, or to point out that spotting and pecking might actually cause problems (like work-hardening or something)?

I am not advising against it at all. The main reason is I don't have any carbide spot drills...yet and I figured the cheap hss spot drills I have might have just work hardened the surface. My logic was to get the tip of the drill into the material and keep it there because I was afraid of work hardening. The chips with the IPT I ran came out continuous and looked great so I probably could do a little deeper holes with this approach but I'm positive at some limit I will have to peck. I just wanted to remove as many options and variables as I could for this first time. I'm sure the quality drills helped a ton too.