Re: Help me quit burning my tools up!
I have been running 304 for the last few days in both the lathe and mill, my first experience with any production run and 304. I found that slower speeds and higher feed rates seem to increase tool life. The stuff work hardens if you look at it wrong, so a more aggressive feed seems to help, avoid tool rubbing.
I found on the mill a speed of about 120 SFM seems to be the best and a feed rate of 3 IPM for the roughing pass, then a finish pass at about 7 IPM with about 0.003 stepover to clean up the pocket. Using a helical tool path to plunge. The pocket in my case 0.727 dia x 0.380 deep, with a 0.450 pilot hole, about 30% stepover. I'm using the knee mill for this project, so flood coolant is not an option, using Kool-Mist coolant in a ''fogbuster'' type system, applied pretty aggressively. Using a 3/8 carbide, 3 flute because that's what I had. Tool life has been pretty good.
I think you are on the right track with your feeds and speeds. One disadvantage you have is the thickness of the material, the center drilling operation may locally workharden the material affecting your boring operation. I found this was a problem when I drilled my pilot holes, I had to increase the feed and slow down the SFM for that operation to keep the edges from work hardening. Maybe using a 135° split point cobalt stub drill to provide the pilot hole (0.245?) and an aggressive feed would be helpful.
On the lathe, drilling with cobalt drills is done at 90 SFM and 10 IPM. Turning is done with proper SS carbide inserts, and running at 260 SFM and 15 IPM, flood coolant. Several hundred parts drilled, tapped, and turned with no tool replacement.
Jim Dawson
Sandy, Oregon, USA