1144 Stressproof Milling with 1/8" endmills

[Galen.Bennett]

I'm currently a student in a CNC machining program and a project we've been assigned is to make a socket for setting pull studs to the right torque spec, and our socket is being made out of 1144. To clean up the inside of the driver side of the socket, 1/8 endmill. It's a 4 flute uncoated solid carbide endmill and we are using a 5/8 long flute to avoid rubbing at the top of the drive when reaching the bottom of the drive which is 0.600 deep. I've turned 1144 before and I know it's really nice to machine, however with an endmill this small and long, I wanted to check with some more experienced machinists to ensure I don't break my endmill the second I start my cuts. I've done most of the roughing with a 1/4 endmill, but to finish I need to get in there with the 1/8. Currently, I've come up 9000rpm at 300sfm, .005 ipt, but with these numbers it comes out to like 180 ipm which just feels disgustingly fast. Does anybody have any suggestions or is that just how easy this material is to machine?

 

[Orange Vise]

.005 ipt,

Way too fast. I'd start around .0005"-.001" for a 1/8" 5xD endmill, and work your way up a bit if needed.

I would also suggest drilling out the corners first with a 1/8" drill, and designing the actual geometry larger than 1/8" so the cutter doesn't get buried.

Depth cuts would be a good idea here. Two or three.

I'd program the stepover at 5% of cutter diameter. If it hums along nicely, you can increase your feed to take advantage of chip thinning, but don't increase the stepover.

Finally, it would be a good idea to add a radius to all of your outside corners.

 

[DavidScott]

Everything that Orange said but I think you should start out around .0002" ipt and 4000 rpm, you can always increase it later. A standard endmill with that much length-to-diameter ratio is iffy at best so be very conservative to start, a 5 fluter would be noticeably stiffer. It looks like you are using Fusion so Adaptive Roughing with clearing out the corners from the previous tool and keep your tool down. I would set the corner radius at .0675" and the blend with the straight sections .02" radius. Sketch it out and only clearance what is necessary, with say .005" of clearance on the corners of the socket wrench. The hole through the center could be bigger too, cutting into the side walls a bit.

 

[Scruffy887]

I would plunge with that .125 a few times per corner. Not sure but it looks like you will be engaging 50% of the radial diameter at 5xD.
But sometimes I also start with a package of end mills to make one part. If I break one I try something else.