Results 1 to 10 of 10

Thread: Fuzzy V-Carved Letters

  1. #1
    Join Date
    Mar 2013
    Location
    Hawaii
    Posts
    13

    Default Fuzzy V-Carved Letters

    I've been V-carving small signs. When the job is complete, some of the letters are not clean. I have to use a toothpick or something to clean some of the letters out. This is AFTER I blow the dust out of the letters.

    I'm using a ShopBot Desktop with a spindle at max speed (18,000 rpm). I use a brand new 60 degree bit. The move speed is the default PartWorks value (3 ips, I think). The letters are .3 inches in height (relatively small). The wood is douglas fir.

    I'm thinking that either the wood is too soft, the move speed is too fast, the letters are too small, or some combination.

    Does anyone know off the top of their head what the problem might be?

  2. #2
    Join Date
    Feb 2004
    Location
    Rogers, Arkansas
    Posts
    1,005

    Default

    It's the doug fir.

    A bit that is dull or not ideal geometry for the material will also create fuzzy cuts. Some vbits cut better than others. I personally like Hersaf v-bits.

    Your move speed is high for that small of letter, but it'll never reach 3ips cutting that small so not the main problem with fuzzy letters. Your rpm is high also unless it's a very small bit.

    For .3" letters, I would run my Hersaf 60v at 14Krpm, 1.5,1.5 move speed, but with the doug fir, not much way to avoid the fuzzys.
    Ken Zey
    Lookout Mercantile / Digital Millwork
    Rogers, AR
    www.CedarSlabSigns.com
    www.lookoutmercantile.com
    www.digitalmillwork.com

    6x12 PRS alpha

  3. #3
    Join Date
    Sep 2009
    Location
    Surrey, UK
    Posts
    1,271

    Default

    You could try a three edge/flute v-bit, some call them engraving bits some call them laser point.

    I only use three flute v-bits these days and I get far better results than I did with the two flutes.

    Ken is right about your RPM's and speeds though.

  4. #4
    Join Date
    Mar 2005
    Location
    Cabinets Plus of Augusta, Hephzibah Ga 30815
    Posts
    1,504

    Default

    also if the wood has a high moisture content it will fuzz

  5. #5
    Join Date
    Sep 2006
    Location
    Garland Tx
    Posts
    2,227

    Default

    I sometimes see improved results by re-cutting the file .005" deeper...

    I also get my best cuts with the CMT three flute "Laser" point bit, however I have no experience with the Hersaf v-bits.

    With small lettering I often put a border around the letters, select the letters and the border to create a V-carve around the letters instead the letters themselves. This helps avoid loosing the small details of some letters.

    SG

  6. #6
    Join Date
    Mar 2013
    Location
    Hawaii
    Posts
    13

    Default Thank You

    Thanks for the tips. Saves me a lot of time. I'll tweak my method with the suggested changes and see what happens.

  7. #7
    Join Date
    Jun 2007
    Location
    Hampton Roads, VA
    Posts
    1,106

    Default

    If I get soft wood fuzzies I will push the fuzz as down as it will go spray some clear on it and re-run the file after the clear cures. Probably too long for production but I will get acceptable results that way.
    "Once a person moves away from the computer and CNC some of the most important work begins." ~Joe Crumley

  8. #8
    Join Date
    Apr 2010
    Location
    Brunswick, GA
    Posts
    192

    Default

    Quote Originally Posted by alan View Post
    Thanks for the tips. Saves me a lot of time. I'll tweak my method with the suggested changes and see what happens.
    Hi Alan,

    You've received some excellent suggestions and perhaps mine will help, as well.

    When V-Carving softwoods such as Select Pine, I always duplicate the V-Carve toolpaths and let them carve twice. I don't go any deeper on the second pass (i.e. the duplicate), but I know some folks do as Steve suggested. I have tried it both ways but have been happier just by running the same toolpath twice...seems to yield a good "cleanup". (I use the CMT "laser-point" 60-degree bit and their 90-degree bits.)

    Also, I have found running the RPM's at 18,000 is good (just like you are doing), but I set the Feed and Plunge rates at only 0.3" per second for softwoods. I think that is the key to my getting excellent results on softwood V-Carves. Even slightly faster at 0.5" per second can noticably reduce the quality of the carve (at least that is what I have observed).

    So, to sum up, try the following and please let me know if it works for you...

    1) RPM 18,000
    2) Feed and Plunge 0.3" per second
    3) Use a great quality V-Bit (I've been using CMT brand, but I'm sure there are many others with similar quality)
    4) Carve each V-Carve toolpath twice (changing depth slightly on second pass is optional, but I seem to get good results without any change)

  9. #9
    Join Date
    Oct 2009
    Location
    Elgin Illinois
    Posts
    689

    Default

    Michael, I too use the CMT 60 degree Laser bit. But one setting I have that is lots different than yours, is the feed rate. I run at 1 inch per second and sometimes at 1.5 inches per second.

    I have a 5HP Columbo spindle, which weighs a lot, on a 5' x 12' PRT Alpha. I get exceptional results carving fancy script letters .25 inches high, as well as large deep v carved letters.

    Going at 2 and 3IPS, I started to get chatter on the side walls of the large V's.

    Even at 1.5IPS, I have files that take 2 1/2 hours to run. If would give up if I had to run at the slow speeds you are running.

    Of course I am sure you have experimented to get your values. I don't know enough to suggest what you may need to do to run at a faster speed. But it would be worth investigating.

    Chuck

  10. #10
    Join Date
    Mar 2013
    Location
    Hawaii
    Posts
    13

    Default

    Hey Michael, I haven't visited since I posted my older reply. I have been busy adding to my pile of live and learn sign failures. I had almost decided to just live with the level of fuzz that I have been getting. I've improved since my first post, but it still wasn't exactly what I had hoped for. Then I read your detailed post and gave 0.3 IPS a whirl. I was ready to take a long coffee break, but 0.3 IPS is not ten times slower than 3 IPS - probably because with ramping and such, 3 IPS is never really achieved. My guess is that setting the move speed to 0.3 took maybe 1.5 to 2 times longer. That would tend to match your results, since my setting of 3 IPS probably only achieved 0.5 or 0.6 in reality.

    Sure enough, the cut was clearly cleaner. I didn't try a double pass yet, but I will soon. As it is, a little blowing and picking after a 0.3 pass isn't so bad - compared to what I was doing before.

    Thank you very much for your detailed advice. I really appreciate the time you took to pass on what you know.

    In case you're wondering, I make 4" x 8" signs with famous quotes, or not so famous quotes by famous people. I've tried pine and douglas fir planks, and I've also tried birch and mahogany plywood. I get the best quality control with ply because I don't have to deal with knots and distracting grain patterns. The only problem is that people generally perceive the plank signs (single piece) as being better than the ply ones. I try to make it up by giving the final product a very smooth, high gloss finish.

    Chuck and Joe, thanks also for your input. Every bit helps.

Similar Threads

  1. Painting v-carved letters
    By Davo in forum ShopBotter Message Board
    Replies: 6
    Last Post: 05-30-2015, 11:59 AM
  2. Jagged Letters Being Carved?
    By NeathawkSigns in forum ShopBotter Message Board
    Replies: 15
    Last Post: 09-09-2011, 07:42 AM
  3. Applying gold leaf to V-Carved Letters???
    By r_jones in forum Sign Making
    Replies: 2
    Last Post: 11-27-2010, 12:18 PM
  4. Painting V carved letters
    By foamman in forum Archives2008
    Replies: 5
    Last Post: 04-18-2008, 12:17 AM
  5. HAND CARVED LETTERS TO CNC
    By larry_k in forum Archives2007
    Replies: 3
    Last Post: 10-27-2007, 06:46 PM

Posting Permissions

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