Machining phenolic (composite) panel

[paco]

I have a request by a new customer for machining part out of phenolic panel (http://www.emcoplastics.com/index.cfm?fuseaction=product.display&product_ID=69&ParentCat=20).

Anyone can help me figuring if it machine well with a CNC router and what cutter(s) is/are best for pocketing and cutting? From Onsrud catalog, the cutter shape vary greatly so I'm guessing each respond to particular phenolic panel type and machining needs.

Also, any particular behavior of the material while machining and what to expect after; does it tear, need clean up of remaining chards and/or fibers...

Thanks in advance for any help.

[don_roy]

Pascal
i just did some phenolic and I found it to be very abraisive and will wear down carbide very quickly. Needless to say I did not make any money. the edges were very clean but I relized it transfered heat right to my table. It is very dusty you really need a vac system. Of coarce it was my first time and I would also like some advise on cutting or just to run away from such jobs.
Don

[paco]

Donald, can you tell us what cutter you used and at what feed/RPM/step down rate/plunge rate and such.

[Brady Watson]

Paco,
These are excellent: Harvey Tool (http://www.harveytool.com/products/search.php?keyword=phenolic)

I tend to err on the conservative side of things. I'd go 1, 0.5 @ 15,000-18,000 RPM and 0.125" per pass. It is similar to milling acrylic (density is similar). You are essentially milling a thick piece of formica laminate. It smells nasty.

Don't be skeered :eek: :D Use those numbers as a baseline and adjust speed & RPM where the machine tells you it wants to be. Observe & listen. Also, ramp into your cuts - no straight down plunges.

-B

[paco]

Thanks for that Brady! So I guess the diamond coating only add to longevity?...

[Brady Watson]

It does a few things...

It resists heat, which protects the cutting edge & keeps it sharp. Plus, it has sub-micron diamond particles that act like fine sandpaper that polishes the edge of the parts.

-B

[bleeth]

FYI: Our typical Acrylic cutting is done with a single straight O-flute running 1.5" per sec at 10-12K. Depth of cut can be pretty hefty. For 1/2" material I just leave a .1" allowance for final cut and have no issues. That being said I haven't cut phenolic tops on the SB but I would probably use the same strategy. The idea of a DLC is quite nice and the 2 flutes wouldn't change my cutting much.Probably go to the somewhat lower side of the RPMs and stick with the rest. Ramping in or slowing the plunge way down (.25/sec) with the Harvey bits seems like it would be totally required. Nice looking bits Brady.

[gripus]

I have cut a number of pistol grips from phenolic, Corian and mesquite wood. I use the same bits, feed rates and spindle speeds for all of them. I have one file that cuts out multiple sets of grips and I will often have a table of blanks laid out with all three materials. I have never had any problem doing that.

I typically run 3.3 ips, 19,000 rpm and .375" depth of cut with a .25" ballnose and a .125" endmill for the profile pass and holes.

Joe