1/8 cutter .600 deep

[mike561h]

I'm having a hell of a time with chatter in the corner redius. It is .0625 and my finish cut is with a .125 2 flute in aluminum. I have tried different speeds and feeds byt no luck. The place i work uses 4 flutes alot. i never used 4 flutes on aluminum.

The operator loaded a 1/2 inch 4 flute for a part i programmed . I had a pocket routine and he wondered why the cutter broke. Well you can't use a 4 flute when you are going 50 ipm and 7000 rpm. I has to set up the job abd run today. The operator has 4 flutes everywhere. I put in 2 flute carbide and ran the part no problem. He also had long length cutters Snap crackle pop. Chatter city. Everything is okay except the radius in the corners. Anyone got any ideas. i could run the damn thing slow and get a GOOD FINISH in the radius BUT JOB SHOPS DON'T LIKE THAT TO MUCH. I WAS RUNNING 13 IPM AND 7500 RPM. JUST SO the cutter would not snap. .550 deep. .125 depth cuts.

[Guest]

I'll agree on the 4 flutes, I use 3, if I can't get 3 I use 2.

 

With a 1/8 cutter that deep, slow the RPM down. If the pocket size allows, use a larger cutter to finish the floor and walls and only use the 1/8 to do a remachine on the corners. I do ALOT of small corner stuff .031R and smaller, that I rough out with 1/2 cutter. Step your corners down using remachine.

 

BTW, on small cutters you DO have ease up on things, the cutters are not rigid enough for the larger cuts. High speed, moderate feed and light DOC's

[mike561h]

how slow. I am using the 1/8 inch cutter just for the final pass on the outside contour .01 . Everything else is finished. i used a 3/16 prior to the 1/8

thanks,

[Lars Christensen]

What about going with a smaller cutter than the radius, so you can actually contuor the radius, insted of you cutter have to take all that stock out at once.??????

[Guest]

An outside contour?

 

Do you really have to use a cutter that small?

 

If there is a feature that requires it can you use a larger cutter and use remachine for the small contour area?

 

Off the top of my head without seeing the geometry, I'd say 10 - 12 IPM.

 

Maybe 3500 RPM

 

If your really going to try to do it one pass.

 

I might try 4 passes at like 45 IPM with a maxed out spindle but if there is an internal radius somehwere that changes slightly, at the RPM you'll likely get chatter.

[Nick_AFRL]

if you have to use a cutter that small ramp it.... we do alot of deep small oring grooves, ramp every one of them less chatter and stress on the tool... works everytime.

[Tim Simmermon]

If you can, play with the tolerance to make the radius a little larger (.010 - .015). This will allow the cutter to walk around the radius a little instead of plunging straight into it.

 

+1 to John on the remachine

[Guest]

I live and die by 3 flute cutters. The asymetrical loading of an odd # of flutes greatly reduces the chance of chatter/harmonics. If I can't find a particular 3 flute cutter, I will keep calling suppliers until I can get one. I'll never settle for a 2 fluter.

 

That said, depending on length and such you should at least be able to run 50-100 ipm at 7500 with the proper 1/2" cutter.

 

.01 is alot to leave for a .125 cutter, try .005. Can you drill corners out (with a .125 drill) to remove majority of stock? When you get in a corner the radius of your cutter your cutting on two sides, really loading the thing up.

 

[ 04-11-2006, 10:22 PM: Message edited by: Chris Rizzo a.k.a.Italian' Stylin' ]

[medaq]

I have had to do .25 endmills down 3.5"'s. The trick for me, I like to releive as much flute as I can. For example with your .125 endmill, Releive it so you have .1-.15 flute length left. And make a bunch of step downs. This way you have less cutter pressure in the corners. I find in the longer skinny tools, they can not handle easily the long flute cutter pressure that gets generated in the corners. So by releiving the endmill your cutter pressures stays constant and as little as possible.

 

Jim

[Rakesh]

I don't know the complete story, If you have chatter at the corner,I tell you the trick. First plunge corners using G81 with 1/8 end mill and if possible stay .002 away from the wall. Than use contour.

 

Best tool is 1/8 chatterless series which 532 series from DEboer.

[c-hook]

I agree with all tht has been said so far, I don't think that .600 is terribly deep for a .125 E.M., But another thing that I do is to use a shorter E.M. to mill down as far as I can, then use the longer E.M to get the deep stuff. By using the shorter tool you can feed alot faster because of the extra rigidity, so in the long run it can save time, especially if you are making lots of parts.

[Kelly Burns]

Id use a contour ramp with high rpms, and moderate feeds (25 IPM) Set the ramp depth at .025 and walk away. It makes a huge difference what your hanging onto the cutter with. I like to use short in holders on something that small. Ive cut .130 slots into D-2 that varied between .50-.75" deep using a 2.5mm OSG cutter. You just cant ram it around so hard.

[88Matt]

sounds like a good canidate for Highfeed. MC will control the feed based on stock removal. You'll need to set up ur machine dynamics at first, but then ur set. the help tab walks u thru it nicely.

[Slixmix]

I always drill my corners out with a drill 1st. Go in there with a .120 drill in the corners to eliviate (sp?) pressure for the endmill.

[heavychevy2155]

i used the drill out the corner trick in 304 ss.

.125 2 flute emill .67 deep it took forever but never broke an emill, I was able to use some of the tolerance 1/64 +- so i went .012 larger radius and no chatter at all .05 depth of cut, 2 finish passes .007 per pass.

[glogg]

i did not read every single post but i would say if you have a 1/8 end mill, make the radius in the database .0630" this way it will be a G03 move instead of just slamming into the corner. it has always worked for me in the past. good luck!

[j.nguyen]

How About A Reduced Shank Cutter .125 Flute W/ .6 Stick Out + What Ever Chris R. Said