Page 1 of 3 123 LastLast
Results 1 to 10 of 29

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

  1. #1
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    57

    Default hardwood profile cutout advice -- my first paying commission!

    Hi everyone,

    I have my first paying commission and am looking to mine the wisdom of the forum.

    I've designed a funky modern curvy bench that will have custom metal legs that someone else is making.

    I cut a short prototype out of scrap 3/4" plywood with pretty good results. But I basically know what I am doing with plywood and a good compression bit, and the client wants it out of 3/4" thick ash. I have pocketed and v-carved ash before with very good results, but I'm worried about all the profile cutouts.

    Here's the bench slat:
    screenshot2.jpg

    And a representation of the little spacers:
    screenshot1.jpg

    They come together to look like this:
    benchprototype.jpg

    For test cuts of the slats and spacers out of ash, I used a 1/4" upcut, .2125" depth 12000 rpm and 3ips, all of which more or less fits with what the SB calculator suggests. The first slat did fine(ish), although that bit really wanted to lift the stock off the table. Indeed, the first spacer got ripped loose and sucked away into the DC system (definitely learned that 1 tab won't do). On the second slat the bit started slipping in the collet and I aborted. I might not have tightened the collet enough, but in any case that leads to my big question:

    How would you approach cutting this job in terms of bit selection, feed rate, pass depth and rpm? Also, edge quality really matters, especially on the top, so climb cut with a .01" allowance and then do a full depth last pass (stick with climb or conventional?)??

    I have an essentially brand new PRS Standard with the 2.2 spindle. I have 1/4" upcut, downcut and compression bits and a 3/8" upcut bit at my disposal.

    I appreciate any advice. I really want to get this cut right the first time!

    Thanks,
    Brian

  2. #2
    Join Date
    Mar 2011
    Location
    Marietta, Ga.
    Posts
    318

    Default

    There is a brand new tutorial on the Vectric Portal website about using compression bits and toolpathing them. I am sure you have an account. Personally, I think 3ips @12000 rpm is a little too fast and too low. I would try 2ips @16000 and see if I am still making chips instead of dust. If your bit is slipping in the collet and it is tight, the collet may be packed with saw dust. Take it apart and blow it out each time you change bits. Hope this is of some help...joe

  3. #3
    Join Date
    Jan 2008
    Location
    Hobby-Tronics, Chiloquin Oregon
    Posts
    1,194

    Default

    EVERY time I think I have ALL the answers, I learn something new! Some of the wood I've been cutting lately is like my arteries, it's really hard and sure is different that the last time I cut it!

    Anyhow, I have shifted to using just a little faster spindle speeds and making a couple more passes that normal. I have also added just a tad to my tabs (a little longer and a little thicker, more tabs is good).

    On those little pieces you might want to not cut all the way through (leave an onion skin) and sand the excess off after the cut. I have a supply of small parts in my DC as well!

    Have fun and good luck on your first for-pay gig! Russ
    AKA: The Train Guy

  4. #4
    Join Date
    Jul 2014
    Location
    Bell, Florida
    Posts
    399

    Default

    I second Russ on both, make more passes and leave a skin on to be sanded off.

    I cut some small parts out of Bass wood (soft) with a compression bit. I bring my material down to just over a half inch, cut depth is half inch, then to the drum sander we go. Sand the back side till they come loose and clean the parts up. I never have them come loose. Hard wood I would use the upcut to keep things cool and clear but would cut shallow cuts so I would not pull the part up.

    Tim
    Tim Lucas Custom Woodworks
    www.TLCW.us

  5. #5
    Join Date
    Jan 2004
    Location
    Marietta GA
    Posts
    398

    Default

    Quote Originally Posted by Tim Lucas View Post
    I second Russ on both, make more passes and leave a skin on to be sanded off.

    I cut some small parts out of Bass wood (soft) with a compression bit. I bring my material down to just over a half inch, cut depth is half inch, then to the drum sander we go. Sand the back side till they come loose and clean the parts up. I never have them come loose. Hard wood I would use the upcut to keep things cool and clear but would cut shallow cuts so I would not pull the part up.

    Tim
    I would use a larger diameter cutter. Looks like you could use up to a 1/2” bit there.

  6. #6
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,548

    Default

    I pretty much cut wood at 3ips 1/4" pass 10k rpms. then a cleanup pass. tabs on wood are a little with the grain are safest but they are the most fragile. on the end grain they are stronger but you risk tearing the grain. so I make them thicker and bandsaw the parts out of the wood.

  7. #7
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    57

    Default

    Thank you to those who responded. I appreciate the advice. I have had some luck in the past with faster, shallower passes with a downcut, which is probably the direction I will go...I guess!

    What amazes me is that there doesn't seem to be any sort of default for through cutting hardwood. If you're cutting 3/4" plywood, for example, a simple default is to use a 1/4" compression bit with 1/4" passes. But there doesn't seem to be such a default with hardwood, especially a harder species like ash. I realize people's machines and spindles/routers can vary drastically, but for the beefier machines with spindles like a ShopBot, I feel like there should be some guidance that's relatively reliable to follow.

    I am having a blast with the CNC...I just had no idea there were so many gray areas!

  8. #8
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,784

    Default

    Quote Originally Posted by bking1836 View Post
    But there doesn't seem to be such a default with hardwood, especially a harder species like ash. I realize people's machines and spindles/routers can vary drastically, but for the beefier machines with spindles like a ShopBot, I feel like there should be some guidance that's relatively reliable to follow.
    Every piece of natural material is different. The grain of the wood, the density and structure varies from board to board. There is no hard rule for cutting natural materials. Only through careful observation and listening to the tool can you dial it in to where it needs to be. Somewhere in the middle is best. Start by picking the feed rate and RPM that gives the best finish and then work on harmonics by adjusting the RPM. Chipload calculators are for maximizing tool life, NOT cut quality.

    Nobody mentioned hold down & how important it is to cut quality. If the part vibrates because it isn't held down firmly, edge quality goes out the window. Also, keep in mind you are routing & not milling...the spindles sold by SB only reach their full horsepower rating above 12,000 RPM. Lower than this and you pull more amps and put more heat into the motor windings. (This also wastes electricity because the motor isn't operating in it's most efficient range. ) Crank that sucker up & route!

    -B
    High Definition 3D Laser Scanning Services - Advanced ShopBot CNC Training and Consultation - Vectric Custom Video Training IBILD.com

  9. #9
    Join Date
    Jun 2017
    Location
    Glendale, WI
    Posts
    57

    Default

    Quote Originally Posted by Brady Watson View Post
    Every piece of natural material is different. The grain of the wood, the density and structure varies from board to board. There is no hard rule for cutting natural materials.
    Thanks Brady. I agree. I'm not looking for a hard rule, just a that starting point -- the "somewhere in the middle" from which I can fine tune. Some people say take 1/4" passes with a 1/4 upcut at 10k rpm and 2 ips for ash; others say 1/8" passes at 16000 rpm at 3 ips with a downcut. Etc. I know there's more than one way to skin a cat, but these are pretty different approaches to achieve the same result!

    Enough people have cut out oak or ash parts on a ShopBot enough times that there should be some sort of best practice starting point out there. As a relative newbie, that's my wish I guess!

  10. #10
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,548

    Default

    oak is like baby wood try purple heart or ipe or suck (G) yes wood likes to vibrate it needs a stronger hold down. here are some tap handles I make out of walnut. I nail between everyone with plastic nails to keep vibes down and cut speed as fast as practical. there is also my air powered clamp for making hollow boxes in a strip. the hose holds the boxes much better and kills all the vibrations I got with the toggle clamps.
    Attached Images Attached Images

Posting Permissions

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