recently we were tasked with cutting an arc in an off the shelf butcherblock top, maple 1 1/2" thick. I purchased an onsrud 52-367 2 1/8" long 1/2" dia. up cut bit. I set it up at 17,500 rpm and 400 ipm. may have been a little fast but since I planed taking 3/8" per pass, I though it would be ok. of course it snapped on the second pass. so I slowed it down to 300 ipm, with a new bit and it snapped after about a foot with a depth of 1/4". what gives? wrong bit? too slow? too fast? not deep enough. thank you

I cut tops like the one you describe at about 70 IPM. Cutting 1 1/2" thick hardwood, I cut in reverse and I would make that cut in three passes with the final cut being about an 1/8". So, my depth of cut is set up for something like .65". I also make sure I remove the cutting shavings from my cut. I slow my bit speed down to about 12,000 RPM, but I don't really know if that is necessary.

I do not have vacum hold down, so having a small final cut makes it much less likely for the blank to move.

You should have no problem.

Another thing I do; For hard corners, like a 90 degree corner, where I might get some tear-out, I put a short line, maybe an inch, offset from my drawing .31" if I'm using a 1/2" bit. I cut these shapes first, that way, there is no tear-out on my corner. I only know my router. These offset lines are open shapes and my bit will travel the center of these lines.

A rougher tool for the first passes will speed it up, or you could use a bit with a chip breaker. If you use a rougher you will need a cleanup pass. How fast, well, I do not have the machine stiffness it sounds you do, but I would expect much better than what you found.

Something like:
https://www.vortextool.com/1465.html

Or
https://www.vortextool.com/1065.html

Don't forget that when you double the length of the bit you cut the stiffness by a factor of four.

Could also be the machine that's flexing and breaking the bit.

Absolutely use a chipbreaker or rougher bit.

Have to be surprisingly careful with long tools. Just cut very shallow cuts and will be fine, and much faster in the end than changing tools etc.
If it would be a production job than obviously finding better suited tooling would be the answer.

Im thinking that the doubling of the bit reducing the stiffness by a factor of 4 is whats going on. I should probably have limited the depth to 1/8" per pass. the machine stiffness is probably not an issue. (I hope, we spent enough on it!)
thank you for the responses

You might want to call CR Onsrud or Vortex if you are doing much of this. Here is a video of a CR Onsrud cutting 2" oak. They are using a 3/4" diameter bit, but they are doing it in a single pass. 1/8" pass seems tedious.

https://www.youtube.com/watch?v=CaSPoE4_VIw

They have an advantage by putting the part on pods and doing a full depth cut - no need to worry about chips packing in the groove.

400 ipm is too fast. Slow it down to 150 ipm at the same rpm. I've done this for years on 1" thick hardwood cutting in one pass with a 3/8" upcut or downcut spiral bit. For thicker material with the longer 1/2" bit I had no problems cutting 1/2" of depth per pass.

You can also go to a HSS bit instead of carbide. At the slower feed rate you are going to be overheating the bit somewhat. The HSS will stand up to the heat better than carbide. Plus the bit will be 1/4 to 1/3 the price of carbide. Breakage is still annoying but less pain for the wallet. In the long run you'll get just as much life out of the HSS bit when overheating is an issue as with the carbide bit.

BH Davis

A rougher cuts more freely. A bigger diameter is a lot stiffer. A worn collet or spindle socket will cause bits to break. If the bit isn't clearing chips fast enough it puts more side pressure on the bit and heat too. Bit shouldn't be too hot to touch after completing the cut. Just slow the feed, 1/2" DOC should be fine. If the bit gets hot, slow the RPM and pay attention to your chip load (look that up in Onsurd's information.)