Results 1 to 15 of 15
Thread: drilling 1" Phenolic
12-20-2011, 12:40 PM #1
drilling 1" Phenolic
Hey folks. Got a few sheets of 1" thick cloth based phenolic. I need to drill 264 holes at least .25" diameter in each sheet. Im trying to accomplish this task on a 7000 Series MulitCam cnc router with a 20hp spindle. Trying to just plunge with almost any style of bit has just resulted in burned up bits. Any ideas on plunge speed or spindle RPM? My current problem seems to be getting the dust out of the hole, causing a heat buildup.
12-20-2011, 12:57 PM #2
I drill 1/4" holes in 16mm Bakelite at 800rpm, 80mm/min and 6 mm pecks. Can you run your spindle that slow?
Hate the smell of smokin' phenolic!
12-20-2011, 01:47 PM #3
Somewhat abrasive material, and to avoid contamination and staining you should run it dry.
I ran the Titex TEC software for organic filled plastic and it suggests this Titex drill, a 3-flute uncoated solid carbide drill A3367-1/4IN, edp# 5154615. Expect at least 4000 holes if you run at 2557rpm, .0059ipr (15.1ipm) feed for a time of 4.71 seconds per hole.
12-20-2011, 02:33 PM #4
If a clean exit on the bottom side of the hole is important, you might want to try a carbide version of a spur center type drill as normally used for woodworking. Any type of drill with a tapered point I ever tried on phenolic would generate heat like crazy because it can flex the material enough to make the hole undersize and then the material closes on the drill and rubs. As mentioned, it does need to be run dry, and its very abrasive hence the need for carbide on any significant quantity of holes.
If you think you're having fun now, you oughta try drilling a half inch hole thru 18" long piece of phenolic round stock. The drill wants to run every which way but straight because the way the fabric is wound in the round stuff makes it very non-uniform so the drill tries to take the path of least resistance and go thru the stock about like a snake.
12-21-2011, 06:50 AM #5
Thanks for the replies. the quaity of hole does not matter as it is just a start hole for a waterjet cut. cant pierce with water, it delaminates instantly. 4000 is the minimum spindle rpm i can get on this machine. Been using an Onsrud 1/4" burr endmill (p.n. 67-012) to some success. It doesnt get rid of heat like it should, but it seems to be a tougher bit than expected. I can get a hole in just 2 plunges instead of 20 little pecks and the bit has survived 792 holes so far. Didnt expect that kind of performance out of a bit like that on this application. Thanks again folks.
12-21-2011, 07:21 AM #6
I'll never get that smell out of my head! Almost as bad as syntactic foam just, not as abrasive.
Do you have the ability to have "through the tool air blow"? It'll make a mess without a vacuum next to the tool.
12-21-2011, 07:24 AM #7
Direct a stream of compressed air on the hole and cutter. Use a length of copper tubing to get right up close and personal.
Blast out the dust, and provide tool cooling.
doug8cat liked this post
12-21-2011, 08:51 AM #8
Got an air stream on the bit already and its helping to cool the bit, but blowing dust out of the hole isnt going to happen. especially since im holding the sheet down with vacuum. the method ive got going now seems to be working fine. Anyone else ever use a burr bit on phenolics? Im wondering how it would cut since it drills pretty well.
12-21-2011, 09:08 AM #9
But SLOW is under 400 RPM in my book - nowhere near 4000. That said, it cuts fast, true and cleanly.
BTW - the fumes from overheat aren't just nasty - they're mildly toxic. Use an ordinary drillpress if they are just starter holes and you can't get that spindle below 4 grand.
TDegenhart liked this post
12-21-2011, 09:28 AM #10
Spindle RPM 16,000
Plunge Feedrate 60 ipm
2 .50" plunges per hole
Its running quick and smooth. The bit doesnt sound stressed, the material isnt burning anymore. I dont think slow is the way to go here guys, not to offend your suggestions. Anyone gotta drill phenolic? Get a burr bit.
12-22-2011, 03:41 PM #11
Handy info, thanks!
Closest thing I have to that scenario is a woodworking router - with carbide. Done a fair bit of thin-section Formica/Micarta edge trimming with it, but based on late 1950's experience carried forward, I'd not have volunteeered to apply it to thicker linen-bakelite 'til seeing wot you've accomplished. Always used slower hand tools to carve that.
N'er too late to learn...
NB: Many of us once made our long, springy, 250 gram layout, punch / riveting / upsetting hammer handles from linen-bakelite - I've put that off for 50+ years as when my turn came I had some 50-year laid-up cherry wood for mine, and it has yet to set a foot wrong.
Last edited by thermite; 12-22-2011 at 03:51 PM. Reason: adding
12-22-2011, 05:44 PM #12
"gotta drill phenolic? Get a burr bit"
Thanks for that info. I had not heard of a burr bit, but will try one next time.
One question- any breakthrough damage?
12-23-2011, 08:02 AM #13
Breakthrough damage-there is just a slight burr on the bottom lip, but nothing that couldnt be easily sanded off. The sheet was vacuumed down to an MDF waste board, so im sure that minimized the chances of de-lamination. Keep in mind that these holes were not drilled for looks or dimensional accuracy. However, the .25" bit did produce holes that mic out at .25" and a clean inside edge.
12-24-2011, 04:12 AM #14
Mcmaster Carr has info laminates including phenolic, you might even be able to talk to someone from the manufacturer and get insider info. My only expirence with it was cutting stripps, wear a mask you don't want to inhale the dust.
12-25-2011, 05:08 PM #15
Carbide burrs are a mainstay in any shop that works with phenolics and epoxy-fiberglass materials. They can be used in high-speed router spindles (overarm type or smaller under-the-table units) for profiling with hand-fed work mounted to templates. Always use them dry with vacuum in that context, especially with fiberglass materials. The actual phenolic grades don't create toxins, unless you seriously overheat them, it's more of a "nuisance dust", to quote the mfr and OSHA data. I spent a fair number of years working around that type of plastic fab. I was glad to get away from it, especially the epoxy-fiberglass stuff. Very annoying.
I'd worry a lot about the end-use product if this is cloth-based phenolic being processed on a waterjet system, as even with the pilot holes, there is still going to be substantial lateral hydraulic pressure driving the liquid into the laminations. Not your problem, I guess.
For the specific hole-drilling application, you've found something that works, so good on ya'. If I were doing that, I might have tried a carbide-tipped twist drill to start, but the big disadvantage you had at the start was the high spindle RPM. I probably would have ended up right where you are, with a burr running at high speed.