Results 1 to 8 of 8

Thread: Baltic Birch Blowout- suggestions?

  1. #1
    Join Date
    Mar 2017
    Posts
    5

    Default Baltic Birch Blowout- suggestions?

    Hi!
    I’m trying to machine something fairly detailed in Baltic Birch ply, using both .125” and .25” spiral upcut endmills.

    The different levels if pockets cut beautifully in MDF, but then this happened with the ply. I’m cutting at 13k, 3 ipm.

    Is it the bit? The Feed / speed?

    Thanks for any help!

    020BEC9E-A126-4232-99F4-BB4B9109D095.jpg

  2. #2
    Join Date
    Sep 2006
    Location
    Garland Tx
    Posts
    2,168

    Default

    “Is it the bit? The Feed / speed?”

    It’s the material!

    A down cut bit or even a compression bit might help. You’re having issues wherever you are cutting across the grain, you could rotate the project 90° and have less lineal inches of cross grain cutting, plus that would make the very susceptible narrow area between the windows, “with the grain” cutting.

    A down cut bit will give you a clean cut at the top of the board but may transfer your problem to the bottom side if your spoil board needs surfacing. A freshly surfaced spoil board will prevent splintering by supporting the wood at the point of cut. A compression bit would prevent the bottom “blowout” but it looks like your rabbet around the windows is too shallow to get into the down-cut portion of the compression bit.

    SG

  3. #3
    Join Date
    May 2014
    Location
    MA
    Posts
    375

    Default

    Steve is right, a downcut will solve that problem. A downcut will have less blowout on the bottom (probably not too much at all if you have a vacuum system).

    Another alternative is to cut the job with two bits. Do the pockets with a downcut and then switch to an upcut or compression for the rest of the job. You probably want to zero off of your table if you do this.

  4. #4
    Join Date
    Mar 2016
    Location
    Brooklet, Ga
    Posts
    183

    Default

    What Eric suggested is what I'd do if I didn't have a compression bit or a down/upcut bit that didn't have a sufficient length of cut. The downcut will push the edge of the top layer of veneer down into the material and the upcut will pull the edge of the bottom layer of veneer up into the material for a smooth surface on both sides.
    2006 PRTalpha 96x48
    3hp SEV spindle
    Vcarve Pro8
    Always eager to consume large amounts of info, tips, and techniques!

  5. #5
    Join Date
    Mar 2013
    Location
    Memphis TN
    Posts
    583

    Default

    I've found that when trying to cut wood that is subject to tear out, using a very small bit like a 1/16" to trace the cuts first solves most problems. The depth doesn't have to be that much, perhaps 1/2 bit diameter. Even dropping to a 1/8" usually prevents tearout. It takes more time but depending on the project, can be worth it. Tracing has the same effect as using a downcut. It provides support for the material under the tracing line. The smaller bits have a lot less force so the strength of the wood vs. the cutting pressure keeps the cut clean.
    ShopBot Details:
    PRS Alpha 96x60x12
    4hp Spindle
    12" indexer
    Aspire
    Rhino

  6. #6
    Join Date
    Dec 2000
    Location
    Thorp, WI
    Posts
    2,572

    Default

    If your pockets are shallow, look for a mortise compression and if you need a clean bottom in the pocket, make it a FEM type. To keep the entry free of tear up, do a profile first with an approach to get the downcut part of the tool below the surface before it gets to the edge of the profile.
    Scott

    If guns kill people, I guess pencils misspell words, cars drive drunk and spoons make people fat.

    "Those who hammer their guns into plows, will plow for those who do not" - Thomas Jefferson


  7. #7
    Join Date
    Mar 2017
    Posts
    5

    Smile

    4F4639F4-6A9C-4F68-B8EA-D1AF42BAE676.jpgThank you all so much!!

    I tried a profile cut first, then used a downcut spiral and it turned out great!

  8. #8
    Join Date
    Sep 2017
    Posts
    2

    Default

    I see that you already found a solution but I wanted to add a couple of ideas for future searchers.

    I had to cut some signs in this material recently and had neither the correct bits nor time to get them. I traced the profile with a V bit first, then ran the file as normal and had very good results.

    There were some through cuts on this same project so I inverted the design and put the face against the freshly resurfaced spoilboard. My visible edges were perfect since the upcut bit was pulling into the plywood from the back side, effectively mimicking a downcut bit. This method doesn't make both sides clean like a compression bit would but it did give the one good side that I needed.

Posting Permissions

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