[plast744]

hi i need help on how to cut deep pocket on 6061 the pocket .75w x 1.75 long x 5.5 depth with .125 rad 4 corner. my plan is too drill out for .125 rad first and
use 1/2 drill drill 3 holes in the pocket to relief cutting. after using 1/2 em with
rough out but i don't know the feed and speed on the 1/2 em with 5.5 long
any suggestion please help thanx you

[BobWarfield]

Deep pocket, eh?

You could start out chain drilling the pocket. Hole drilling is often the fastest way to remove material. Or you could just pocket it down in layers. I kind of like the idea of at least doing the pocket corners with a twist drill, perhaps insetting them to leave room for a finish pass. Corners are where you hit maximum cutter engagement and would typically want to slow down on a job like this.

Whichever way you go, chip clearance is going to be key on this job. Make sure you have at least a strong air blast to clear out the chips running continuously.

For such a deep hole relative to cutter diameter, you want a carbide endmill. They're much stiffer. Take it easier on depth of cut too so as not to load it up to much with side forces.

Something else to consider is using the largest diameter endmill you can--they're stiffer. For a 3/4" wide pocket, you can sneak a 5/8" in there and it'll be stiffer than the 1/2".

How are you planning to program the pocket? Do you have a CAM program, or will you write g-code by hand?

Try to avoid full slot cutting as much as you can. Ramp down or spiral down and then just cut less than 1/2 the full tool diameter depth of cut as you move around the pocket.

G-Wizard comes up with the following feeds and speeds for 1/2" 2 flute carbide endmill:

- 4600 rpm
- 36 IPM

I would dial down the feedrate about 20% (that's a Hanita recommendation) since you're going deep, so maybe try 25-30 IPM.

If you can't use flood cool, be sure to get some WD-40 onto the cutter (to reduce chip welding) and go with the strong air blast.

Cheers,

BW

[plast744]

thanks for the advise. on 5.5 in long em cutting would it be to fast at 4600rpm.
when cut deep pocket, my main concert it chatter. i will try it at the speed first. we have camworks system
on cam

[BobWarfield]

Yup, where the chatter sets in is going to be the question. You'll almost certainly find some. If I got chatter, I'd be inclined to reduce the feedrate before reducing the rpm though. And I'd reduce the depth of cut before I reduced the feedrate.

Cheers,

BW

[DareBee]

wow

I wouldn't consider taking on that pocket with a mill unless my customer was willing to pay for failure.

I really want to know how it turns out and how you make it work.

I would, however, take on the job and burn it in the EDM.

[gibbsman]

For a deep pocket like that, I like to use a stub length carbide endmill with a long shank that has been relieved for the DOC required; it is much more rigid then having an endmill with a long flute length. I would usually use an endmill smaller than the corners so i can interpolate them to reduce chatter but in this case it might be best to use the same size endmill as the corner rads and plunge them at a reduced RPM first. When side milling, if you experience chatter do not reduce the feedrate but the RPM, it is better to increase your chipload. Destiny makes an exceptional tool for aluminum, it is ground to reduce chatter & works well on low RPM machines.

[kwhizz]

Ram EDM...........

Ken

[RICHARD ZASTROW]

Find an old Fart like me who has a shaper or slotter. He should be able to cut your corners square with a square tool. But then you'd have to put a CNC control on it to qualify for the 'Zone. LOL

Dick Z

[Andre' B]

I would tell the customer if he works with me and redesigns the part to be easier to make he gets price A if not price B. And B will be very much more then A.

[tizm]

Try going in with a 5/8 3flute carbide em.I would use a lower rpm and higher feed,that will reduce chatter.you will probably have some chatter that deep no matter what.depends on whats exceptable to your cust.I also like the idea of drilling out the corners 1st.If not,then you can ramp down from end to end.