Bore or Circular toolpath

Hey guys!
Quick question, I am making a bushing out of bearing bronze . my question is how would i get an accurate bore. Im not sure the best way to do this in fusion 360. it seems like once i do my finish pass my machine ramps way up and it doesnt make an accurate bore. should do a bore leave radial stock then come back with a circle toolpath at the end ? My cam skills arent the best, im still learning. anyways the tool im using is a 3/8, 3 flute haas EM, and im using bearing bronze stock and the bore size is 12.5mm . so i guess my final queston would be can i interpolate this or will i need to drill and ream ? thanks guys!

Honestly, I would bore to within around .002 and then use a reamer if the inner dimension is that critical.

Ideally this is lathe work.

a boring head is the best way to go on a mill but they are pricey for good ones. What do you mean by ramps up? And how do you mean inaccurate? A helical tool path will give the least deflection but it shouldn’t matter too much as long as your finish pass is tiny like .005 or less. If it chatters slow feed or switch to helical if it’s not already or take less stock for the finish. Nothing wrong with a slow feed rate unless you need to make a million. 10-15 ipm should be fine for finish pass, used your sfm calc or testing for rpm that provides best surface.

Agreed this is definitely lathe work. And when i say speeds up i mean the feed goes up but after reading yojr post im thinking my feed rate may be too high im thinking it ramps down at my ramp feed of 15 then it does the finish pass at like 25 which with the tool dia being so close to the final size i think thats where my issue lies. I need to slow the actual feedrate down also not just the ramp speed. Does that sound right ?

I agree this is lathe work. But, if you leave the bore .002 oversized. A ream of the correct size is the way to go.
With that being said. I cut bores out with the mill that are dead nuts on. A final finish pass at 10 ipm or slower.

Sweet ! Ill slow everything down and give it a shot ill update everyone as soon as im done

1 Like

Yeah just slow it way down, Can even go down to 5 Ipm and work up from there. Sometimes fusion bumps feed for finish passes but definitely want to knock it down for this. The large endmill in small hole Can really make it worse for sure.

Okay, so after taking everything into account slowed down to 10 ipm for the bronze and realize 12.5 was to big so i went down to 12mm. I left two thou of radial stock and did a fully separate op for finishing and it came out at 11.99 which i think will be just fine for my application. Just for fun i made the same part out of 4140 PH and slowed everything down to 8 ipm and had almost identical results. Im extremely happy with the results. I think for the sake of time im going to get a drill and ream it will be so much faster and easier on the machine. Thanks for all the help guys!