Page 2 of 3 FirstFirst 123 LastLast
Results 11 to 20 of 29

Thread: hardwood profile cutout advice -- my first paying commission!

  1. #11
    Join Date
    Jun 2013
    Location
    Pasadena, CA
    Posts
    947

    Default

    Maybe I missed it but is this job a one-off, small series or larger series production? Your speed/feed/bit size optimization strategy may depend, also how you hold it down. For small quantity the tabs may be O.K. and the feed etc. is not that critical because you will spend anyway more time preparing and finishing. But for larger quantity of all the little blocks I would probably drill/mill the holes first and make a custom fixture with suitable dowels to hold the parts for the cutout (downcut bit) without tabs.

    As for the final product, you may have to somehow chamfer the sharp edges or they could leave unwanted patterns or splinters on users' posterior.
    Box Joint, Dovetail, Guilloche and MazeMaker Software Here

  2. #12
    Join Date
    Jan 2011
    Location
    gleason, wi 54435
    Posts
    408

    Default

    Those small parts in hardwood can be a pain even with good vacuum hold down. If I were doing this job I would run these as fast as possible and leave a large tab (1 inch wide .25 tall) on one of the straight sides. Make sure the vectors were straight lines of coarse , then run the parts through a table saw to remove the tabs. For safety have the parts on the off side of the blade so you don't pinch them with the fence.

  3. #13
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    98

    Default

    Quote Originally Posted by Burkhardt View Post
    Maybe I missed it but is this job a one-off, small series or larger series production? Your speed/feed/bit size optimization strategy may depend, also how you hold it down. For small quantity the tabs may be O.K. and the feed etc. is not that critical because you will spend anyway more time preparing and finishing. But for larger quantity of all the little blocks I would probably drill/mill the holes first and make a custom fixture with suitable dowels to hold the parts for the cutout (downcut bit) without tabs.

    As for the final product, you may have to somehow chamfer the sharp edges or they could leave unwanted patterns or splinters on users' posterior.
    At this point it's a job that I will run only a few times. I never thought about a jig or fixture for this. Very interesting idea. As for people's posteriors, I plan to ease the top edges of the slats with sanding sponges. It will also get a spray lacquer finish, which will help.

    Ultimately I'd like to iterate the design to eliminate all the small spacers -- which I think is possible with two long slotted slats that run perpendicular to the main slats in place of the spacers. But I have to figure out how to transfer the geometry and create some sort of notches so that everything lines up.

  4. #14
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    98

    Default

    Quote Originally Posted by bobmoore View Post
    Those small parts in hardwood can be a pain even with good vacuum hold down. If I were doing this job I would run these as fast as possible and leave a large tab (1 inch wide .25 tall) on one of the straight sides. Make sure the vectors were straight lines of coarse , then run the parts through a table saw to remove the tabs. For safety have the parts on the off side of the blade so you don't pinch them with the fence.
    Great idea about the tabs and TS. A 1" wide .25" high tab in ash should hold pretty well. I like using the bandsaw to get through tabs, but I'm working with larger stock than usual for this job. Thanks.

  5. #15
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,560

    Default

    or taller and shorter like 1/8" long and .5 tall or more thats easier to sand. that pic I posted has those tabs .

  6. #16
    Join Date
    Dec 2011
    Location
    Rapid City, SD
    Posts
    623

    Default

    Great thread - cool jigs - I love the air hose clamp idea!

    I just completed a project that involved flip-ops for 64" long, arc'd 8/4 hard maple strips. 2" wide with 1/4" groove down the center on both flat faces. First time in 6 years running the machine that I had to do flip ops. Used clamps on ends of the rough stock and set dowel pins in table for flip alignment.
    What I learned:
    Forget the tabs. Leave an onion skin .125 thick - ( think "full tab"). Radically improved cut quality - just need to go to bandsaw for a quick release of parts from rough stock. High quality flush trim bit to clean up.
    1/4" bits are to be abandoned with this density and thickness of lumber. Chips jamb/burn /packing = slipping and broken bits. 3/8" is essential for harder woods. Use a chip breaker bit if you can.
    Up-cut is probably best. Still had a few jambs with a compression, leading to packing/burning of chips on a few pieces.

    Good luck!
    Jeff

    Wish I'd heard Brady's comment sooner about the RPM's to power. I've been fooling myself thinking I'm babying the machine keeping things at 12k or lower. Works for plys, but will try higher RPM's on future projects.

  7. #17
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    98

    Default

    Quote Originally Posted by jTr View Post
    What I learned:
    Forget the tabs. Leave an onion skin .125 thick - ( think "full tab"). Radically improved cut quality - just need to go to bandsaw for a quick release of parts from rough stock. High quality flush trim bit to clean up.
    1/4" bits are to be abandoned with this density and thickness of lumber. Chips jamb/burn /packing = slipping and broken bits. 3/8" is essential for harder woods. Use a chip breaker bit if you can.
    Up-cut is probably best. Still had a few jambs with a compression, leading to packing/burning of chips on a few pieces.

    Good luck!
    Jeff
    Thanks Jeff! I can foresee projects where that approach would be really helpful. This time, I am pretty much stuck because I started today. Got the ash all lined up in VCarve and on the spoilboard and drilled all the 3/8" and 1/4" holes, as well as 33 hold down screws! I ran out of time so I left the computer and shopbot on, and tomorrow morning I will do the through cuts. I am holding my breath.

    IMG_2906.jpg

    After I read your post I went back into Vcarve to see if I have room for the 3/8" upcut to do the through cuts. It's possible for the bench slats, although it's tight and I worry about the integrity of my tabs/hold down. A 3/8" bit is a no go for the spacers. Is it worth trying just for the slats?

    If not, my strategy will be to use a 1/4" downcut at .16" deep passes, starting at 2.5 ips and 12k rpm. I will adjust feed and rpm on the fly based on sound. For better or worse, I've broken enough bits that I can identify the warning sounds.

  8. #18
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    98

    Default

    Quote Originally Posted by knight_toolworks View Post
    or taller and shorter like 1/8" long and .5 tall or more thats easier to sand. that pic I posted has those tabs .
    I think this is part of the answer for me today. Thanks!

  9. #19
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    98

    Default

    Update for anyone who might be interested....I cut one of the ash panels this morning -- the one with 64 spacers and 2 slats. I used the 1/4" downcut at .162" passes. Ran at 2.5 ips and adjusted rpm to 12500 up from 12000 during the cut. It screamed a bit, as 1/4" bits do, but it cut without incident. Edge quality is decent.

    spacers.jpg

    The narrow, tall tabs (.25" x .65") worked quite well. No issues with parts rattling or coming loose. I placed them on the back and bottom of the pieces where any residual after sanding essentially won't be seen anyway.

    So now I have the remaining 30 slats to cut. I didn't love how it sounded when the first two slats were cut on the first panel...I wonder if I need to slow the feed rate down. The spacers were fine at 2.5 ips, but they are so small that I doubt the machine ever actually went 2.5 ips. I'd switch to the 3/8 upcut but I just don't have enough room for adequate and proper holddown.

  10. #20
    Join Date
    Apr 2013
    Location
    Kennebunkport, Maine
    Posts
    3,927

    Default

    For kicks and giggles,
    If using a climb cut with the downcut...swap to a conventional profile pass.
    Most of my downcut bits prefer it on profile passes.
    Feed is in the ballpark, tweak rpm's and then increase both proportionally until quality suffers...then I usually back off 10%.
    Like everyone has been saying...Listen to it
    2 cents.
    scott
    Scott Plaisted
    2013 Desktop/spindle/VCP 9
    Maine

Posting Permissions

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