Originally Posted by
Brian L
Swath,
Some of that was almost painful to watch.... especially the boring head. OK, first, I'm not sure where you are getting your feed and speed data, but you are off, by quite a bit.... too much rpm in just about all of your cases and not even close to enough feed rate.
I don't know what size of an endmill you are using to profile your barrel part, but it looks to me like it might be a 1/2" diameter and you are trying to profile 3" deep. If you only want to make say under 20 pieces, struggle along any way you can.... if you want to make these fast and efficiently, you'll have to change things up.
First, start with a "normal" length 1/2" endmill, it'll have 1" depth of cut, go around your part until it won't reach any longer, then get an endmill that will reach the length you need, but, with a 1/2" flute length, a long shank and reduced diameter shank, i.e. it will measure .490" or so while the endmill cuts .500". This will be worlds stiffer, and given you are only taking fairly shallow depths of cut, it'll work much better.
Then at the end, if you have to, use your full length endmill.... now, here, I don't know what your tightest corner radii is, but if it's .25, then don't use a 1/2" endmill, you want to never "bury" it into a corner, you want to be profiling at all times, so if the radii is .25", then try to find a 7/16" or preferably 3/8" endmill to finish with.
Speeds and feeds..... rough numbers..... first lets talk feed, it should never be less than about 1/100th of the diameter of the endmill, so for 1/2" it should be .005", and that is per tooth.... so if you are running a 4 flute it will be .020" per revolution, given your 2000 rpm I saw most of that running at, you should be feeding closer to 40 ipm.
Now, I think your rpm's are too high also, but hey, if you ain't smokin' endmills, more power to you. We figures aluminum and brass... wide open, give it all she has for rpm... with carbide, you won't get too fast.... think we used to figure 600sfpm for HSS in aluminum. For mild steel carbide drops back to about 200 sfpm (roughly), given some of the better coated inserts, that could be 400, but for your run of the mill carbide endmill, again, unless it has special coatings, 200 is a good ball park. You said this was 4140ht, so I'd back that number down to maybe 150 to start with.
Once you have your rpm and feedrate, your hp is extremely limited, so you will have to vary your depth of cut and step over to accommodate the hp available. You will find once you have the right rpm and feed, you will be cutting the material off rather than rubbing and chattering like you are now.
I know it takes a leap of faith and it's a butt puckering moment to plow right in there, but you'l find out in short order the tools will work better and the machine will remove metal faster when things are dialed in. You will break a few tools learning what you can get away with, but in short order you will know what will work.
Oh, the boring head it's a rare instance you can spin one over 500-700 rpm... try backing that puppy way down and see what happens when you try to bore a hole... you should get a long, continuous stringy chip..... usually makes a bird's nest all around the tool... then it's cutting like it should.