Results 1 to 10 of 10

Thread: Inlay help

  1. #1
    Join Date
    Apr 2008
    Location
    John How Guitars, Cool California
    Posts
    32

    Default Inlay help

    I just got my buddy up and running, attached the spoil board and made it flat using the tool. So for my first project, I decided to cut a pocket in which to inlay my logo which is just my two initials in script. I imported a jpg file into partworks and made a toolpath for the inlay pocket and then made a toolpath with the same file for the logo profile.
    Next I cut the parts on the bot and everything went great except the logo doesn't fit in the pocket. It's close but no cigar. I'm sure I can play with it to get it right but I'm hoping there is a built in factor that I can use to make the two fit. Anyone know if there is a scaling feature or some kind of fudge factor for this in partworks? I am using a 1/32" spiral upcut bit for this part in case it matters.
    By the way it was very fun and exciting finally getting the tool moving after having it sit in my shop for the last month while I worked up the courage to get started!!!

  2. #2
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,623

    Default

    it is trial and error because it will depend on the material and the bit and how fast you cut and how tight you want it and if there are sharp corners on the inlay piece. doing it with a vcarve inlay for smaller pieces can be easier.
    the best way is to use a tapered bit then the pocket can be a bit large.

  3. #3
    Join Date
    Mar 2006
    Posts
    7,830

    Default

    check this out:
    http://vectric.com/forum/viewtopic.php?t=564
    it looks like a inlay tutorial post type thing

  4. #4
    Join Date
    Apr 2008
    Location
    John How Guitars, Cool California
    Posts
    32

    Default

    Thanks guys, Jack, they are doing some very fine inlay with this procedure. I will look at it a little closer.
    Thanks!!

  5. #5
    Join Date
    Oct 2000
    Location
    Willis Wharf, VA
    Posts
    1,643

    Default

    Paul has written an article for the ShopBot wiki on his inlay technique...it refers to VCarvePro but works the same with PartWorks

    http://shopbotwiki.com/index.php?title=VCarveProInlay

  6. #6
    Join Date
    Aug 2005
    Location
    Vectric, Alcester
    Posts
    147

    Default

    John,

    For a simple 2D inlay you need to remove the sharp corners from the vectors before you cut them out.

    If you imagine a simple star shape, when you cut the pocket the tool is not going to be able to get into the sharp outer corners and the tool radius will be left there. When you cut the male insert with a profile cut, the tool will not be able to get into the sharp corners on the inner points of the star. This means that the two pieces wont fit together regardless of any allowance needed generally.

    The trick to getting rid of all the sharp corners is to use the vector offseting tool.

    Assuming you are using a 1/4" diameter tool (radius 0.125")

    1) Select your vectors and offset OUTWARDS by 0.125" (the tool radius)

    2) Delete yor original vectors (or move them to a new layer)

    3) Select the offset vectors and offset INWARDS by 0.25" (the tool diameter)

    4) Delete the vectors you created in step 2) as no longer needed

    5) Offset the vectors created at step 3 OUTWARDS by 0.125" (the tool radius)

    6) Delete the vectors you created in step 4

    You should now have a set of vectors which match your original vectors but all internal and external corners less than the tool radius will have been replaced by radii which match the cutter diameter.

    I hope that makes sense!

    Brian

  7. #7
    Join Date
    Mar 2008
    Location
    Tulsa Oklahoma
    Posts
    1,237

    Default

    Brian- that is an excellent explanation of the procedure needed to make the inside and outside radius's match the bit.

    Don't you wish PartWorks just had a tool to do that for you? Hint, Hint, Hint.

    After doing it manually a few times it gets old, and is done so often by so many people it should be made part of the design software.

    D

  8. #8
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,623

    Default

    yes vcarve inlay works well. I did a regular inlay I did a test piece with the same toolpath and the two fit fine do it on the good wood and they inlay was a bit too big.
    a tapered bit will do a lot it will work more like vcarving but not have the size limit.

  9. #9
    Join Date
    Feb 2006
    Location
    USAF, CA
    Posts
    29

    Default

    Have a process thats roughly same as described in preceeding posts. I use a 3 degree tapered spiral bit. I intentionally make the inlay a bit larger, glue, tap it in then sand flush. Makes for a perfect fit - no gaps. The trick is finding the correct offsets.

  10. #10
    Join Date
    Apr 2008
    Location
    John How Guitars, Cool California
    Posts
    32

    Default

    I appreciate all the helpful comments. I was originally trying to use a small straight bit because I wanted to make pockets for some existing shell parts. I will still pursue that but in the meanwhile I used the procedure posted above and came up with this version.
    here are a couple pics.
    inlay and pocket
    Completed inlay

Similar Threads

  1. Inlay toolpath
    By Kyle Stapleton in forum ShopBotter Message Board
    Replies: 7
    Last Post: 12-17-2014, 04:09 PM
  2. inlay
    By genek in forum Project Ideas
    Replies: 2
    Last Post: 06-19-2013, 05:27 PM
  3. INLAY OFFSET ?
    By tim_mcknight in forum ShopBotter Message Board
    Replies: 3
    Last Post: 04-30-2009, 12:53 PM
  4. Cutting inlay with the PC.
    By betacrash in forum Archives2008
    Replies: 10
    Last Post: 11-25-2008, 11:21 AM
  5. Floor Inlay
    By brian_harnett in forum Archives2005
    Replies: 7
    Last Post: 06-29-2005, 09:01 AM

Posting Permissions

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