I have a chatter problem on my mill I need help with. I have a 4000 pound bed mill with box ways and a Bridgeport style variable speed head. I'm trying to machine out an oval pocket in 3 inch thick 6061. I rough out the part with a roughing cutter with good success (2.2 inches deep). But when I change cutters to a new 3 flute 1 inch Aluminum cutter (installed in a new good quality single set screw nmtb 30 tool holder) I always get chatter. The depth of cut is only .1 inches. I've tried to vary the spindle rpm and feed rate but the problem never totally goes away (3600-1000 rpm / 35-.5 feed rate). I machinery dealer familar with this machine told me to increase my Rpm and feed rate but this only seams to make things worse. The mill ways appears to be in excellent condition. I see little wear on the machine as a whole. I changed all the bearings in the head (only high quality bearing were used). The mill now sounds a lot quitter but the problem is still there. I could email pictures to anyone willing to help. My pictures are too large to attach to this post.
We do lots of holes in 6061, 2" and 2-1/4" deep with smaller cutters; 1/2 running at 10000 and 5/8 running at 7500. My experience is that a new tool is always more likely to chatter but the chatter diminishes and dissappears after a dozen parts or so. I have my guy play with the speed and feed overides. Generally it is a case of backing off on speed or increasing feed; the intent being to increase the chip load. It is possible all you need to do is wait for the cutter to "wear in". I have sometimes put a chunk of scrap in and take some nice heavy fast cuts to get this done rather than have the chatter on good parts.
But I also have this image in my mind of a 1" cutter in a 4000lb machine; that is a small machine and I wonder if you are operating past its limits.
Heres my 2 cents.. The 1" cutter is pretty big for R8 and 30 taper tool holders. Not saying you cant have success with them but I would downsize to a .625 EM (preferably carbide) with 1.0 loc and 2.25 stick out from the holder. You want your set up to be as rigid as possible. So you will need to spin back your EM to 2.25 length to give clearance and prevent galling. You should be able to take 1" depth of cut on a finish pass in aluminum depending how much you left for stock. You may try using a 2 flute EM. Usually 3 and 4 fluters have less chip clearance than a 2 fluter and essentially your increasing the size of your chip by slowing down your rpm and speeding your feed . This should help you with your chatter.
Your simply asking too much form the cutter and the holder for that depth..what you should do is take a couple of steps and a clean up pass. You should be able to hit .045 maybe .050....if your lucky but .1 is way too much for that length
Thanks for the suggestions. I reconfigured the program for a 3/4" 2 flute cutter (the smallest I had with the reach I need). The first cut was at a depth of .38" the chatter was still bad with a varied speed and feed. The first programmed speed was 2050 RPM at 24 feed. When I mentioned .1" in the original post I meant depth. Would it be worth while to buy a longer reach 1/2" cutter and retry the cut? Is the first cutt too deep?
You should be able to take way more than .375 depth of cut on your finish pass with a .75 em. There could be a number of factors here why your getting this chatter. How much did you leave for your finisher? I would leave .005 to .015 for a finish pass. Is your quill sticking out to far? Make sure your as rigid as possible. Does your part need an extra clamp to make it more secure? Whats your flute length on that 2 fluter? Find a .75 em with 1 inch of flute length and the remaining 1.25 all solid shank( spin it back if you can for clearance) and step it down till you get to your 2.2 depth You would be supprised how rigid the tool is like this. Your walls wont be as tapered eather than trying to cut it with a tool that has long flutes. Maby try cranking your rpm down a bit more too if your using HSS. Hope this helps.
If I'm reading the Niagara Cutter chart correctly a 3/4 em cutting 6061 should turn 1500 - 7000 rpm. This is based on a sfm of 500 - 1500 and a .005 per tooth load. My cam program set the speed and feed I mentioned in the last post. I used the rpm and feed overrides to try and find a working combination but no luck. The feed was varied from .5 too 30. The speed I varied between 1500 and 2200 rpm. I have a hold-down clamp on each of the 4 top corners of the part.
are you feeding clockwise or counterclockwise around this oval shape. is the cutter "squealing" loudly with vibration, or does it sound normal and just end up rough. is the oval through the part or is it a pocket, if its a pocket are your chips coming out of the pocket when cut, or falling back in
The feed is ccw in a pocket. I would have to say it is squeling loudly with vibration. The chips are doing a little of both. But there does not seam to be a problem with the chip compacting or being cut multiple times.
You could be getting "spindle stretch" as we call it,Bad retainer springs slightly loose preloaded spindle bearings poor retention knob- collet ball retainer. Part lift from the vise.
One old trick (I should know as I am Old ) get a right hand cut left hand helix cutter and try it.
You will probably be surprised at the finish as all you tool preasures are into the spindle and pushed down into your part.