Acrylic: Drilling Holes and Newbie Questions about Feed formulas

Results 1 to 4 of 4

Thread: Acrylic: Drilling Holes and Newbie Questions about Feed formulas

  1. #1
    Registered
    Join Date
    Jan 2009
    Location
    USA
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Acrylic: Drilling Holes and Newbie Questions about Feed formulas

    So, I have a CNC router, and I'm somewhat constrained on the variables at my control presently. Namely, I am limited to a spindle RPM between 10k and 23k, and a maximum feed rate of 80IPM.

    We'll get to that in a moment -- but, as a newbie, I have a (very important to me) equation to figure out before I really get started routing acrylic. I'd like to get feedback on it _before_ I start to avoid the same mistakes I made in wood ($40 in bits broken in 5 minutes == a stop to any work until the next payday).

    So, my question is pretty straight-forward: I need to cut a number of small holes (think 0.196" and smaller in diameter) for screw pass-throughs, I have a 1/8th single-flute up-cut spiral bit, and a whole slew of drill-bits. For holes like the the .196", would it be wise to use just a standard drill bit (knowing I bottom out at 10k RPM), or to use the 1/8" carbide router bit?

    So, in that light: should drilling in acrylic be done by drill-bits, or by router bits? In whichever situation, does anyone have any advice on plunge rates?

    To the constraints I mentioned earlier, everyone out here seems to like very low spindle speeds and moderate feed rates, or very high spindle speeds and exceptionally (to my limited budget at least =) high feed rates. I'm a bit confused, as when I calculate out for the "optimum" rates, using the formula on plasticrouting.com, I always end up with something in the range of my machine... That is, given I'm forced to choose one of the factors, I choose RPM at 10k, and if Cl = Feed/(RPM * CuttingEdges), and I'm using a single-flute helix, and an optimal range (according to the above website) for Cl is 0.004 to 0.012, I get Feed == 0.008 * (10000) == 80IPM. Of course, as 80IPM is my "maximum" speed, I consider that I could tune for "worse" finish (theoretically) and choose 0.006 which gets me closer to 60IPM, and staying well away from my upper limit and relaxing the possibility of positioning errors.

    But why do I get such drastically different ranges using that formula than what people talk about on here, and shouldn't bit size play a role in the formula? I.e., shouldn't my 1/4" bit be able to be pushed faster than the 1/8" bit?

    Thanks for any advice!

    !c

    Similar Threads:


  2. #2
    Registered
    Join Date
    Apr 2006
    Location
    USA
    Posts
    187
    Downloads
    0
    Uploads
    0

    Default

    How thick is the acrylic you're putting holes in? Given your machine the two flute carbide 1/8 " bit should do nicely. Try the holes at 11k/50 IPM. If it's thick acrylic peck the holes and keep the bit clean, blow it off with compressed air if you have it. Routing edges might be a problem at 80 IPM, you may have to make a few passes depth wise, melting the acrylic might be an issue at that slow speed, maybe try 14k rpm.



  3. #3
    Registered
    Join Date
    Jan 2009
    Location
    USA
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default

    Thanks for the advice, I'm primarily dealing with .25" and .125" cast acrylic sheet, making small housing for electronics and mechanical components. Most parts will require all of: facing (part cut-out with tabs), pocketing (creating groves for panels to slide together, and counter-sunk holes), and straight drill operations.

    For keeping the bit clean, at the moment I am stuck with hand-holding the ol' shop-vac, as until I complete the enclosure, I can't have acrylic dust all over my office, getting into computers and printers and such. (I realize the contradictions here, but I mean "I like to keep it reduced" vs. "blowing it all over the place" =)

    Thanks for the info - note: I have only single-flute cutters, I presume those would work fine as well? (They are Onsrud 63-744 and 63-712)

    !c

    Edit: I think I figured out why I was confused by the formula, namely, that it was only part of the equation (i.e. it gave me IPM, but RPM had to be "guessed"), I found this link through another post on here, and it cleared everything up for me: http://www.cyro.com/methacrylates/MC...ef5Routing.pdf

    In light of that, it looks like I can get pretty acceptable values at 15k RPM and 60IPM, yielding a SFM of around 340 or so, and an IPT of 0.004".



  4. #4

    Cool Re: Acrylic: Drilling Holes and Newbie Questions about Feed formulas

    Realizing this is an old thread, but may come up on someone's search for information..... Here's some information that may help.

    1) Drilling holes in acrylic / polycarbonate (or similar) sheet: Use drill bits for holes that are specific for acrylic. Tip angle should be either 60 or 90 (preferred) degrees as opposed the the standard jobber drill bits that have 118-130 degree angles. The sharp tip helps cut in better without cracking. SPEEDS: Spindle speeds should be as low as possible. The smaller the hole, the slower the spindle speed. We run into similar problems as others: We can only go as slow as 4K RPM on the spindle. So if your spindle speeds can not go below that, slow your IPM for the plunge as much as possible. I usually run about 4,200 rpm spindle (for holes up to 1/4") with a plunge speed of 26-32 IPM. Seems slow (and it is!), but you will get really nice holes. As noted, a good backer is needed. Spoil board is good, just don't do it in a spot with an existing hole larger than the one you're drilling. (You'll blow out the other side more often than not.)

    If you want to route acrylic / poly carb material.

    Acrylic will cut very nicely using Onsrud bit #56-625 (1/4" o_flute, straight) or X-Edge bit # XO-2912 (1/4" Down spiral O-Flute) We use those 2 tools on the majority of acrylic/PC material up to .25" thick. RPM is usually around 14-16,000, feed is 160-220 IPM. Adjust for thickness and edge quality. (I'm still working on getting a nice "flamed" edge on the router and haven't quite gotten it yet.

    If you run into a situation where you need to cut polyethylene (HDPE) or polystyrene (PE), a good compression bit does the trick for me. (X-Edge XC-2022-M or XC-2023-M / 1/4" or 3/8" coated for long tool life.)

    Hope that helps anyone else that may be looking to process plastics of sorts.



Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Acrylic: Drilling Holes and Newbie Questions about Feed formulas

Acrylic: Drilling Holes and Newbie Questions about Feed formulas