milling deep pocket

[barnesy]

I am trying to mill a pocket with a wall depth of 67 mm in alum. with a 20 mm hss long series end mill .THe tool is getting a fair amount of chatter ,which would be better climb milling or normal and what depth of cut would get the best finnish

[Karl_T]

The DOC you can use is dependant on how rigid your mill is. Sounds like yours is not rigid enough Try smaller cuts. You are using a very sharp two flute endmill?

Plunge milling might work better for you to rough out the pocket.

Climb milling gives a better finish.

Karl

[barnesy]

I only have 2mm left all round the pocket the size of the pocket is 666x209
the cutter has 4 flutes

[Karl_T]

In that case, I'd turn up your RPM for the finish cut (maybe 750-1000 or more), climb mill, use coolant. Good luck.

Karl

[subtrek]

Take multiple depth passes and break up the amount of the cut, also u may want to try a 3 flute mill or one of the variable pitch mills these are great for chatter problems. The last thing might be to try making the same cut using different speeds and feed combinations to find the so-called sweet spot, this comes usually by really upping the RPM or Chip load.

[JPMach]

Try using a solid carbide cutter with eccentric relief

JP

[big_mak]

Some of these long cutters can be sort of too sharp and tend to grab. If this is a HSS cutter, take some 600 grit. Run the cutter in reverse and just give the edges a little tickle. This can be just enough to get rid of the chatter.

Another trick is to relieve the endmill, so you only have say 10mm of cutting length, then take 9mm deep cuts. This will lessen the contact of the tool and equalize the pressure on the side to reduce deflection.

Once you get into these long series endmills speed and feed rules don't generally apply. You need to tweek speeds and feeds to your particular setup. Holder, endmill, machine, and material. These speeds can vary when any of the variables change, including the machine as rigidity of each machine is different so it's basically an experiment.

[dertsap]

i agree with big mak on all his suggestions ,
2 mill is an awfull lot of material to leave for a finish cut especially when using highspeed
now assuming this is being done on " cnc ?? " then i would suggest less material for the finish cut no more than .25mm and ramp the walls at roughly 3.17mm depth this way you will have a constant steady pressure on the tool where as the contant lead in lead out will cause possible gouging chatter etc , as well as show the lead in points ,,high speed and high feed ,
and snug up the tool ,dont have anymore stick out than is necessary

[barnesy]

Have finnished m/c pocket it worked out fairly good and I was very happy with the end result (so was the boss ).I ended up taking full depth cuts of .2at about 750 rpm and a feed of 350mm ran the final cut cut twice .I left 2mm under size so I could get a feel for how it would go,only left .5 on second end as I had to shift the job The finnished pocket was 1246 long 209 wide M/C only has 1000mm tavel but it worked so I am happy .Thanks for all the suggestions