Trying to cut .043 slot in 01 tool steel breaking endmills Help

Ok so I am new to this and just got my CNC (x2 mill DIY converted to CNC, MACH3 and Fusion360) working my first project. So I am trying to cut .043 hole in 01 tool steel. For practice I have been playing with 1/16" cold rolled steel plate. I had luck using a .043 Colbat Endmill cutting this slot so I thought I would try the tool steel. 1/16" tool steel plate. I was using like 2000 rpm at 3IPM feed. Broke 2 of these Niagara cutters. So guys whats the answer? I sure appreciate the help!

A difficult project. A wire EDM would be my first choice for this job, but I'm assuming you don't have one in your back pocket.

O1 tends to work harden if you don't have enough feed speed. But using a 0.043 endmill limits tooth load, I think cobalt is a good choice. Right now at 2000 RPM and 3 IPM translates to a surface speed of 23 FPM and 0.0008 tooth load (assuming a 2 flute end mill). My gut says that you are turning way too slow for a 0.043 end mill and should be up around 6000 RPM, about 60 SFPM in O1, but I have no data to back this up. I have cut quite a bit of O1, but never with an endmill that small.

I would try drilling a series of ~1 mm holes to remove as much material as possible then maybe plunge mill with the endmill with about 20% step over. Then run a finish pass to complete. I don't know if Fusion has a plunge milling cycle, but you can manually make that happen, even hand code the cycle if needed. Using a 0.043 endmill in a 0.043 slot eliminates the possibility of using adaptive clearing so you are going to have to get creative.

Quote:

---

Originally Posted by Jim Dawson

A difficult project. A wire EDM would be my first choice for this job, but I'm assuming you don't have one in your back pocket.

O1 tends to work harden if you don't have enough feed speed. But using a 0.043 endmill limits tooth load, I think cobalt is a good choice. Right now at 2000 RPM and 3 IPM translates to a surface speed of 23 FPM and 0.0008 tooth load (assuming a 2 flute end mill). My gut says that you are turning way too slow for a 0.043 end mill and should be up around 6000 RPM, about 60 SFPM in O1, but I have no data to back this up. I have cut quite a bit of O1, but never with an endmill that small.

I would try drilling a series of ~1 mm holes to remove as much material as possible then maybe plunge mill with the endmill with about 20% step over. Then run a finish pass to complete. I don't know if Fusion has a plunge milling cycle, but you can manually make that happen, even hand code the cycle if needed. Using a 0.043 endmill in a 0.043 slot eliminates the possibility of using adaptive clearing so you are going to have to get creative.

---

Don't think fusion has plunge milling cycle, but easy to model. Pattern along path. To make the tool path quick, model a tiny hole, small enough to not over lap with the 20% or whatever needed step over, pattern along path with stepover as spacing, use a drilling cycle, select one hole then check box for select same diameter. Automatic plunge milling cycle.

Very shallow passes is also an option. 10 or 15 thou at a time and there should be no issue