What's new
What's new

diamond bits for machining G10 sheet

Chris999

Hot Rolled
Joined
Feb 11, 2005
Location
Vancouver B.C.
Looking for some recommendations on manufacturers for 1/4 or 3/8 dia bits for machining 1/8 and 3/16 thick G10 sheet.

Thanks in advance.

Chris
 
What kind of #s? Do you want carbide or diamond? There is a new add on the home page banner for carbide routers from YG.
 
When I was doing this I used an insert end mill that used three TPG221 inserts, which I got from Valenite.

These were PCD (polycrystaline diamond) full length inserts.

Carbide works OK but the glass fibers pick out the cobalt binder in the matrix, and the carbide
particles fall out eventually. PCD lasts a lot longer.
 
Guess I should have added more detail. It's milling shapes out of G10 sheet and slotting G10 square tube.

Curently using carbon coated carbide, 5k rpm at 40 ipm. Eats endmills like nothing else I've seen.
This stuff is Evil.
So a diamond coated end mill / router bit is what I'm looking for...
 
I just went the opposite.

Cheaper carbide, because then you are just wearing a cheap tool and it doesn't sting

Don't do as much as I used to, but did quite a bit

Essentially, if you are wearing the tool out you are probably spinning too fast.
G10 you tend to not be able to hold well, so that is your feed limitation.

I am running a 3/8 or maybe 5/16 carbide end mill, might be coated, at 4500 rpm, 38 ipm.

We trace out a part in 1/8 FR4, about 19 inch perimeter, 100 at a time. Not a new end mill[probably recently did a bunch of fussy bearing counterbores in 110 6061 parts], and I am sure we don't kill it in the job. It of course would need to be replaced to do anything fussy, but it certainly could do some more in G10/FR4.

I'd have to look it up, but what is that, a 30 dollar end mill. 100 parts.

If you are trying to do something fussier than +- .005, or not able to hold it well as the load goes up with a less than sharp tool I can see that.
 
Guess I should have added more detail. It's milling shapes out of G10 sheet and slotting G10 square tube.

Curently using carbon coated carbide, 5k rpm at 40 ipm. Eats endmills like nothing else I've seen.
This stuff is Evil.
So a diamond coated end mill / router bit is what I'm looking for...

Slow your sfpm down. We run G10 all the time, and just get our endmills,drills and taps "diamond" coated from our resharp guy and they last a LONG time. I run my tooling around 200sfpm in this crap.

I put diamond in "" because I don't think they charge us much to have them coated and they don't look like your traditional big brand diamond coated end mill.
 
I asked my guy this morning, 3 flute 3/8 solid carbide, coated with something or other
Ok you made me look MSC 80230634 Ticn coated, 59 bucks.
we ran 100 of a part that uses this tool a lot in aluminum, and while finish is not critical, we don't want a burr

then we ran the g10 with it

then we ran 100 more of the previous part

300 parts, .20 a part

and it might have been in before, and it is still in the machine, last purchased in october

SO if tool life is bugging you, either you are spinning too fast, or you need to rethink your parameters.

On a side note, all tools, cutting tools to hammers, run 1 percent of my expenses.

I haven't had anything reground in decades. when it is dead, it is dead
 








 
Back
Top