Help me quit burning my tools up!

I've been boring holes with a .250" carbide endmill into stainless steel tubes (304). The wall thickness is roughly .035" I put a center drill hole there first to help keep from having 'caps' at the end of my tool when it goes to do the next hole. Either way, the end hole is a .257.

I'm using an endmill to help keep the inside of the from getting a lot of nasty chips. I'm putting 4-6 holes in each tube, depending on which part I'm doing. I'm running at 1800rpms and Feeding at 1ipm. My tools are going quickly, and end up building an aggressive set of chips fairly quickly. I've tried nearly doubling those speeds and feeds, which has less chips, but doesn't help my tool life at all.

*edit* changed to 1530rpms & 1.5ipm plunge, 3.0ipm on linear

Chips seem better, not sure about tool life yet

Any suggestions?

P.S.
I work in a very small shop, we have 2 Fadal 2016 VMCs. I am limited to end mills & drills, no fancy tooling. We have carbide, that's as fancy as we get.

Thanks in advance!

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.

A question for the pros: is boring a 0.257" hole with a 0.250" tool essentially the same as drilling? Would it make sense to choose a smaller endmill?

Quote:

---

Originally Posted by CitizenOfDreams

A question for the pros: is boring a 0.257" hole with a 0.250" tool essentially the same as drilling? Would it make sense to choose a smaller endmill?

---

Maybe. You can cut more aggressively with a larger end mill and in this case that's important. Removing as much material as possible with a drill bit is normally the most efficient method. I also avoid plunging with an end mill where possible, there are exceptions to this, like when you can plunge with less the half of the end mill diameter contacting the work.

In this case, I would drill leaving maybe 0.010 or so for the finish pass so the endmill can get a bite without rubbing.

Plunging stainless like that is hard on an endmill. I would probably use a carbide drill and around a .234 drill and then mill using a 3/16 or 7/32 carbide EM. No center drill since you are milling it after drilling. Run about 80-100 SFM on the drill, and your speed & feed should work ok for the finish. You could also use a HSS drill instead of carbide, but I would run that at 40-50 sfm.

I've found uncoated carbide works ok at 100sfm and .001ipt, and coated carbide works well at 200sfm and .001ipt in 304. The coated carbide endmills will outlast uncoated endmills, and are worth the extra expense

Thanks everyone!

Uncoated Carbide 4 flute 30 helix.

I'm using 100SFM with .0005" IPT.

Still running @ 1.5IPM plunge - 3.0ipm linear. Seems to be the 'good spot'