Chatter in the Corners of a Deep Box

[MetalMarvels]

I am about to loose all my hair on this one.....

 

I have an aluminum box to make - 3 inches wide, 5 inches long and 2-1/2 inches deep. The walls - before roughing out the exterior - are about 1/2 inch thick. The corner radii are R.250 for the full depth of the box then the first 1.17 inches are relieved to a radii of R.125. I am getting the material roughed out just fine - leaving about .030 on the side walls to clean up (and R.750 in the corners) using a 2-inch shell mill to blow the chips out. I have been using a long reach, releaved shank 1/2 dia four flute to finish roughing the interior to about .002 of material left for finish. The problem that I am having is finishing the interior - particularly the corners. I have tried ramping in with a 7/16 dia four-flute (3 inches of cut). I have tried a straight contour. I even tried a 3/8 Dia extra length in the corners.

 

Basically the side wall finish sucks and the corners are worse. I haven't had a lot of experience with deep sidewalls like this. I thinking of clearing the corners with a 1/2 dia drill first..... Any ideas??

 

EDM (I wish) is not an option.....

[Jack Mitchell]

Gary,

 

Cut the rpm back to about 25% of what it is that you are using; manually overriding the feed rate at the corners will also help immensley. Trust me - this is going to work out - ultra low rpms for any and all extended length of cuts.

 

P.S. - go with a two flute if possible; the thought behind such foolishness is that the fewer teeth involved with the cut will render the better finish.

 

 

Regards, Jack

[MetalMarvels]

Thanks Jack. I am currently running the 4-flute 7/16 dia at about 1000 RPM with a feed of of about 12 ipm. So I should drop this to about 750 RPM and about 9 ipm??

[Jack Mitchell]

I think you responded while I was editing. Please have another look; don't be shy - cut it back to 400 rpm - this will work.

 

6" is a deep pocket to me in H13 or 4140HT; when you get pinned with this type of work you have to learn to be adaptable and to overcome the chatter. I would not even consider 100 rpm too slow on this length of cut.

 

Good luck.

 

Regards, Jack

[MetalMarvels]

darn....

 

I sort of got hung out to dry on this one - Must be done by Monday and my only other choices are a 1/2 dia 3-flute and a 1/2 dia 4-flute that are long enough to reach. I do have a 7/16 dia 3-flute serrated edge rougher - but somehow I don;t think that one will work too well for a good finish...

 

Would ramping down the walls be better than a standard 2-pass contour (or more passes to take out the spring) at a slow feed/low rpm? The only problem with the ramp is dying of old age before it finishes..........

[Rekd™]

Also, you might drill the corners before you rough the pocket. You can get brave and drill right to net finish in the radii, or go small and leave a small amount of mat'l for the EM to run over at VERY low RPM.

 

Another thing might be to machine the corners/walls to about +.003 to .005, then take the EM and drill it into the corners at net finish, again with low RPM, them come back and finish the walls.

 

Let us know how you do.

[Bruce Caulley]

We do deep pockets with small corners in Aluminium regularly and only use high helix 2 flute tools. These let you keep the revs quite high compared to a 4 flute standard helix tool.

 

Bruce

[MetalMarvels]

BC - I do have a nice 1/4 dia two flute high-helix extended reach (a Javelin I think) that is doing a good job for me in the R.125 ares - unfortunately it isn't long enough to get all the way down....

[Jack Mitchell]

3 flute 1/2" cutter with three "Z" passes will do the trick.

 

Low rpm with a fast feed - take care to override at the corners and be sure to do a small circular interpolation on these corners as well.

 

This is not the tough job you are anticipating; holding a .0006" tolerance across a 6" depth of cut is difficult and whether you believe me or not - it's obtainable.

 

Hang in there - you are going to ace this job.

 

P.S. I never ever liked a 7/16 end mill regardless of depth of cut - clearly my least favorite among many - but that might be the bad taste left over from snapping them four fluters off in aluminum of all things.

 

 

Regards, Jack

[MetalMarvels]

Thanks! I now go forth to grapple with this aluminum brick once more!!! At least I have lots of stock for a change. Now if I only had a chip conveyor.........

[MetalMarvels]

Just noticed - my post count is stuck at 456.... Does that always happen when you start the thread???? wait - they incremented. - sorry - case of "D'OH" here......

 

getting late I think....

[Jack Mitchell]

Screw the post count - just get back in here on Monday and tell us all how you made 10K on the weekend and need help finding some guys to take for beers.

 

Regards, Jack

[Teh Bear without Brains kinda idiot]

drill corners(drill it with your end mill too ) ,low rpm (up to 20-30 % of recomendations or less )and rather high feed and conventional instead of climb .

climb pushes mill into the wall ,conventional out of the wall .

HTH

[MetalMarvels]

Right you are, Jack! Better than a 16u finish and bang on for size as best I can measure it. Looks nearly polished. I had to put a couple of M0's in to clear chips, but other than that, working great. The highfeed with finish only worked great for entering and exiting the corners at a much lower feedrate - no singing at all!!!

 

Thanks! I usually drink wine myself - but I know where to come up with a couple of six-packs of your favorite!

[Guest CNC Apps Guy 1]

I'd go with the drill in the corners myself also. With that kind of Depth:Diameter Ratio, e/m'ing that is gonna be a byotch!

 

JM2C

[d00d]

opps

[d00d]

+ 1 On drilling corners, sometimes I squash the wire from deep pockets to different construction planes and after hoging out and create larger radius' (sweep) and work the contours up in cuonstrution planes and down to size accordingly. So you would have your original radius at 0 depth, say it's a .5, at construction plane.200 I'll squash the radius up and make it a .560 and cut with 1.00 mill. then step down each time. But only cut hard steel here, may not apply to aluminium

[MetalMarvels]

They are turning out great now - mostly had to back WAAAAY down from my usual aluminum speeds and feeds. Using the highfeed option and going into the corners very slow was another important piece. Drilling the hole in the corners works well too - I drilled them about .005 under size. As I mentioned earlier, I am getting better than a 16u finish now - with no measureable taper (measureable that is with what equipment I have and certainly well within +/- .0005).

 

Thanks for all the help! Now... Who is stopping by for a beer?

 

[altaeng]

Use a good tool.

Data flute 3fl aluminum finisher or.

Dura mill.

Viper.

Hanita.

Drill out corners.

Use remachine to semi finsh corners.

Pocket finish floor.

Then finishwalls.

But its your tool.

[SLJ]

We usually "drill" the corners with the finish E/M after roughing, and offset center enough to leave a couple of thousandths each direction. "Usually" works fine.

[Shawn Wentzel- Wenteq Inc]

what speeds and feeds did you end up with? What was your max feed and how slow did you go in the corners?