Results 1 to 15 of 15
Like Tree2Likes
  • 1 Post By CalG
  • 1 Post By thermite

Thread: drilling 1" Phenolic

  1. #1
    alhauger is offline Plastic
    Join Date
    Dec 2011
    Location
    TEXAS
    Posts
    7

    Default 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.

  2. #2
    NeilJ is offline Plastic
    Join Date
    Jul 2008
    Location
    Melbourne, Australia
    Posts
    31

    Default

    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!

  3. #3
    PixMan's Avatar
    PixMan is offline Diamond
    Join Date
    Jan 2007
    Location
    Central MA USA
    Posts
    4,528

    Default

    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.


  4. #4
    metlmunchr is offline Diamond
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,286

    Default

    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.

  5. #5
    alhauger is offline Plastic
    Join Date
    Dec 2011
    Location
    TEXAS
    Posts
    7

    Default

    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.

  6. #6
    Road HOG Mill is offline Plastic
    Join Date
    Jan 2007
    Location
    Milwaukee / Gurnee
    Posts
    33

    Default

    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.

  7. #7
    CalG is offline Titanium
    Join Date
    Dec 2008
    Location
    Vt USA
    Posts
    3,540

    Default

    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.

    Cant hurt!
    doug8cat likes this.

  8. #8
    alhauger is offline Plastic
    Join Date
    Dec 2011
    Location
    TEXAS
    Posts
    7

    Default

    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.

  9. #9
    thermite is offline Diamond
    Join Date
    Sep 2011
    Location
    Mid-Atlantic USA, South China
    Posts
    11,363

    Default

    Quote Originally Posted by alhauger View Post
    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.
    Worked linen-bakelite for years - still do - at SLOW speeds with either the right sort of woodworking drills (Forstner bits) or with milling cutters - always dry. Cobalt or carbide only on glass-filled laminate.

    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.

    Bill
    TDegenhart likes this.

  10. #10
    alhauger is offline Plastic
    Join Date
    Dec 2011
    Location
    TEXAS
    Posts
    7

    Default

    Current feeds-
    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.

  11. #11
    thermite is offline Diamond
    Join Date
    Sep 2011
    Location
    Mid-Atlantic USA, South China
    Posts
    11,363

    Default

    Quote Originally Posted by alhauger View Post
    Current feeds-
    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.

    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.

    Bill
    Last edited by thermite; 12-22-2011 at 03:51 PM. Reason: adding

  12. #12
    NeilJ is offline Plastic
    Join Date
    Jul 2008
    Location
    Melbourne, Australia
    Posts
    31

    Default

    "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?

  13. #13
    alhauger is offline Plastic
    Join Date
    Dec 2011
    Location
    TEXAS
    Posts
    7

    Default

    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.

  14. #14
    doug8cat is offline Stainless
    Join Date
    Jul 2008
    Location
    Philadelphia
    Posts
    1,489

    Default

    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.

  15. #15
    specfab is offline Hot Rolled
    Join Date
    May 2005
    Location
    AZ
    Posts
    809

    Default

    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.

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •