machining copper

[billystein]

I am getting ready to start a copper job. Can anyone recomend cutting tools? Carbide or tool steel. also will be using side mills. any help on speed and feed?

[Jim at Gentex]

All I can tell you is knock your speed / feed down 15-20% from where you would cut aluminum...and use LOTS of coolant. The material tends to gum up on cutters. Other than that, have a ball!

 

[Teh Bear without Brains kinda idiot]

As a roughers I use 3 fluets hogs solid mills for alluminium ,for hog mill 12 mm S7500 f2500 z step 4 mm or s6000 f2000 take-off 6 mm ,bigger feed possible ,but my electrode holders will not stand it .

Also I like 3-4 flueted end mills end mills with coating for middle cuts and finish.

for end mill 3 mm S8000 (my maximum spindel speed ) f1500mm/min

z step 0.5 mm

For surfacing I use 3-4 fluets mills with extra-short fluet length with coating ball mill 6mm s7000 f2000 ,ball mill 1 mm s8000 f500 .

Try to use good tooling ,avoid radial bitting ,use a lot of coolant ,try to avoid using HSS mills .

If your relation length/diameter more then 10

do not be afraid to drop speed ,avoid shrieks in the corners .

I prefer Iscar coating IC900 and YG Xpower

For end mill 0.3 mm without coating S7850 f50 zstep 0.06 mm .

for big electrodes I use bull nose round corner insert mills from seco ,

for seco bull nose 25 mm radius of insert R6 2 inserts s7000 f7000 z step 0.7 mm

 

HTH

WTHH

[Code_Breaker]

Run like 7734 . . .

 

Actually, cobalt tools hold up great because of the transference of heat . . .

 

Code_Breaker

[Dan_AKA_ROY]

Never machined copper, so I can't suggest anything.

 

One point to make, though: Make sure your wear eye protection. A copper speck will burn and hurt like hell. It will flare up if caught in your eye until removed.

 

I had an aluminum chip I needed a doctor to remove once. Thats when he told me to watch out for copper.

[TheePres]

BillyStein!!!

A name from the past.

[cvomooney]

what grade? OFE or some alloy and is it dead soft or aged i.e. 1/4 or 1/2 hard.

dead soft is by far the worst it gets better with age...

 

when drilling take most of the releif out... or it will grab. I never use split points on copper.

 

as far as feeds and speeds, use about 75% of what you would use for aluminum.

[JAMMAN]

I remember doing copper on a lathe, it was soft but without a good flood would stick to tn coated carbide no problem.

 

I agree with the zero rake drill bit no center relief. Much slower rpm than aluminum worked for me.

 

In a press I have sharpened round punches with 4 relief angles meeting in the middle, ejector pins didn't seem to help much. Again in a press plenty of lube. This particular material was half hard for an electrical bus duct.

 

Good luck!

[cvomooney]

My favorite cutting fluid on copper is A-9.it's green and messy but it really works great.

[billystein]

Hi Press,

Nice to hear from you. I heard you left the farm again. Are you still @ AOL?

 

Billy

[billystein]

Thank you everyone. I will report what I learn.

 

Billy

[Keith Graydon]

Copper is very abrasive. Lotsa wear on HSS tooling.

[GVM]

We run quite a bit of copper. Try and use TIALN coated carbide whenever possible. I start at 500 sfm for a .5 dia. 2 flute cutter approx. .003 chip load or 23ipm feed. With drills I prefer 15 deg helix you can push them harder. Example .125 drill 9000 rpm 17 ipm feed. Much flood coolent.

[BernieT]

If customer allows it, use Telco copper. Machines almost like aluminum.

[Harryman]

Form Tap!!!