Cutting Copper?

[robtown]

I need a V bit capable of cutting copper (.080). Any suggestions??

[paco]

Hi Rob!

How about a metal chamfer bit (not tipped off ones)?
From your post, I guess your looking for cuting with a chamfer... right?... or engraving?

[robtown]

hey Paco,
Yep, looking for a beveled thru cut, or chamfer cut on some .080 copper. I've done some testing with a 90 degree v-bit I had laying around, edge quality was not terrible, but I'd like to do better.

[paco]

Rob,

what's your observations so far; burr(both sides?), ridges, else...?
Are you cutting dry?
How fast? Stepdown?
Does the material OR the router/spindle chatter while cutting?
Pics?

[robtown]

Chattering on the north side. Obvious tool marks on the ends and the south side.

Spraying wd-40, it doesn't seem to get hot at all.

Speed - started at like 0 and worked my way up to .6

Tried the router at 10,000 and 13,000rpms

stepdown - .02

I do think there is some chatter, but I didn't do much in the way of holddown.

I'm an idiot, I let the customer walk out of the shop without getting a picture of it.

Overall the guy was happy with the two samples we did. He didn't mind the edges because they were to be hammered and patina-ed anyway.

I will get pictures and post them ASAP...

[Brady Watson]

Rob,
If not taking pictures of cool stuff you made on the bot before the customer takes it away, makes you an idiot....then I am the heavyweight champion of idiocy...I let a lot of really neat stuff leave the shop without pics...the issue is almost always that the batteries are shot or the camera grew legs!

In regards to machining copper...sounds like you are in the ballpark if the cutter is not gumming the copper. Another little trick is to pop the copper in the freezer if the size of the material allows it, before machining.

When machining any type of metal, a good hold down setup is essential. The fact that the copper is soft tends to make it absorb a lot of the vibration. A vacuum setup would be in order to hold the piece down if doing multiples or DS tape if you felt it would do the job. The ridges may be coming from the material not being held down with enough force...and could also be that your V-rollers on the X and Y cars need to be adjusted tighter via the cam adjuster bolt on each one. This made a difference on my machine when doing some plastics recently. Adjusting the rollers a bit tighter eliminated a lot of the chatter that I was getting.

-Brady

[dvanr]

Just a thought , when you cut thin metal are you mounting the metal to the table or elevating it 3 or 4 inches?

I would expect that if you mount metal closer to the underside of the x car that you would reduce the leverage that the work exerts on the carriage through the z axis. Might get rid of some of that chatter.

DvanR

[Mike Windsor]

I've v carved engravers brass ( sometimes called trophy brass ) using a 60 deg engraving bit ( flat on one side ) at at a feed of.6 running a pc router at 20,000 rpm no lubrication. The engravers brass is a soft aloy and easy to cut . I used vacuum to hold the sheet with duct tape around the edges of the sheet .One of my projects is at http://www.windsorboatworks.com/new%20racer/P4030014.jpg

[paco]

Impressive Mike!

How was the V tool after?... was it still healthy!?

What was your stepdown?

Did you got burr?

[robtown]

Thats pretty sweet. An edge like that would be sublime on this copper...

R

[gerald_d]

Mike, it looks like you did both the engraving and the edge with the same cutter? How thick is that plate?

[Mike Windsor]

the plate was .125" thick . I used VM 5 to create the file . The profile was cut at a stepdown of .008 with the same cutter, leaving the last .003" uncut to hold the vacuum . I then cut the part out with a knife .

[robtown]

Fortunately I managed to turn out a prototype nice enough that the client returned for some actual pieces, and this time I got pictures...

Copper sign plates, chemical etched and cut on a prt with a 60 degree chamfer end mill (thanks Paco)


4734
4735

[paco]

WOW! Awesome!

Where did you choose to get the bit?

How was burring?

How well copper cut at thoses RPM? What was your last feed and plunge, stepdown, etc... on thoses last parts?

I happen to have some copper sheet scrap (1/8" Thick)... I might try myself too soon...

[robtown]

Hi Paco,
sorry for the delay...

I purchased two 60 degree camfer end mills from McMaster Carr, one with two fluts one with 4.

Burring was a bit of a problem as it left a little sharp edge on the tops and bottoms of the cut. Nothing a few minutes with a file couldn't handle.

I cut at 13,000 RPM (PC router) and went .04 each pass (2 passes on .080) at .9 ipm, don't remember the plunge speed, I didn't make any changes there so it's whatever the 1/8" Alum setting is...

I took a scrap piece of solid surface material and screwed it down to the spoilboard, and double face taped the copper down (double sided masking tape) and sprayed a little wd-40 in there from time to time.

It all worked out pretty good. Something I found out about cutting copper is that the shavings are small and have sharp edges.

[paco]

Thanks for the infos!