Results 1 to 9 of 9

Thread: Fixing 90* V Carve Font Serifs

  1. #1
    Join Date
    Sep 2016
    Location
    Eastern Virginia
    Posts
    70

    Default Fixing 90* V Carve Font Serifs

    I wanted to carve this with a 90* bit and wasn't sure it would work. Looking at the preview in V Care Pro looked like it "might". So I took a shot. It's really marginal, and after painting and sanding I'm not sure that what is there of the serifs will still be there. Probably not likely. I was debating going back over it with a 60* bit. I need to do that with the "fire" anyway as the "points" at the tops of the flames didn't come out at all. Anyone have any other suggestions as to how to make the serifs just a little deeper/wider while keeping the 90* text before I redo it all with a 60?

    The attached is the preview. I couldn't get a good picture showing the outcome since my phone refused to focous on it up close.
    Attached Images Attached Images
    ShopBot Desktop 24x18
    Spindle
    VCarve Pro 8.5xx

  2. #2
    Join Date
    Apr 2013
    Location
    Kennebunkport, Maine
    Posts
    3,758

    Default

    Walt,
    Maybe go off workpiece and MZ,-.005 and zero Z there...and if a little more is needed LIE a little more?
    I'd probably do only 1 letter with the smallest interior "island" and test first to see if it gives you what you want. .005" really shouldn't be too noticeable if it doesn't.
    Scott Plaisted
    Desktop/spindle/VCP 8.5**
    Maine

  3. #3
    Join Date
    Sep 2016
    Location
    Eastern Virginia
    Posts
    70

    Default

    Thanks Scott, I had thought about something like that, but I was thinking of just changing the toolpath start depth to something like .005 or so and then going from there. I don't want to make the rest of the letter too much wider/deeper though, they look really good as they are. So I'm not sure .005 would be enough to make a difference in the serifs and then much more might mess up the look of the rest of the letter. I knew when I picked this font it would be tricky. Now I'm rethinking myself, again.
    ShopBot Desktop 24x18
    Spindle
    VCarve Pro 8.5xx

  4. #4
    Join Date
    Dec 2000
    Location
    Thorp, WI
    Posts
    2,493

    Default

    I keep harpin' on this one, but people just can't seem to come to understand it. MN (Move Nudge) and click the down arrow (for negative or down) on the Z axis, to the desired amount (-0.005 in Scott's example), hit enter, done, re-run the file.

    Another option that I use often is to apply a slight offset to the font. Group it and use that for the new toolpath. How much depends on the font and size, but start at 0.008 - 0.01.
    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


  5. #5
    Join Date
    Jan 2004
    Location
    Norman, Ok
    Posts
    3,075

    Default

    V Carving is one of the most delicate techniques and sometimes not that well understood.

    While this technique can quickly produce a beautiful carving, it's tricky. In order to be successful one needs to get started with clean vectors. You want to avoid drawings with lots of nodes. Scanned images can have tones of these and will seldom render properly. Cheap fonts can be a real heart break since they don't have intelligent nodes. For example, a circle or oval shouldn't have but four.

    Bit depth is critical.
    The crispness and sharp corners need to be maintained. If the bit is too deep the image looks sloppy and crude. Getting those beautiful delicate lines can be a challenge. For that reason I often make the first pass a little too shallow. Then place a business card under the corners of the substrate. It's a fast way to keep going. I've even lifted one side of a panel that's cutting a bit too shallow.

    Everyone needs a 120 degree v bit. The drawing below was done with one of those.

    Joe Crumley


    Last edited by joe; 02-16-2017 at 06:40 PM. Reason: Photo didn't convert

  6. #6
    Join Date
    Jan 2011
    Location
    gleason, wi 54435
    Posts
    371

    Default

    You need a good flat spoilboard, and a parallel blank. In my opinion painting the sign and then sanding away at the sign face doesn't give great results especially on fine detail. Better to mask the blank, paint through the carved mask, and then peel.

  7. #7
    Join Date
    Apr 2013
    Location
    Kennebunkport, Maine
    Posts
    3,758

    Default

    (Scott, Thanks for "Harping"! Think it sunk in this time My brain sees "nudge" and reminds me of one of my very first Spacebar Pause/Nudge during a Z move in 8.14, and the subsequent bit DIVE that spooked me Thanks again for a real simple time saver! scott)
    Scott Plaisted
    Desktop/spindle/VCP 8.5**
    Maine

  8. #8
    Join Date
    Sep 2016
    Location
    Eastern Virginia
    Posts
    70

    Default

    Thanks for all the tips and suggestions. Before I did anything else I somehow realized I had carved with the V bit setup as an engraving bit by mistake ( I setup my V bits as both engraving and V and I picked the wrong one). I'm still not 100% certain of all the differences between a V bit being setup as an engraving bit vs a V bit, excpet I know when you set it up as an engraving bit it knows if there is a flat, of which this particulat one is .006. I had learned before by trial and error that if you use it as an engraving bit it doesn't carve as deep as if you use it as a V bit. So I changed the toolpath and recarved it using it as a V bit. A little bit better, and a lot faster. On the smaller text at the bottom I then went back and went down another .008". Better still. I think I can get away without sandng out the details at this point. As for the paint mask, I have yet to try that but it is on my list of things to try. Still new to all this and learning and trying new and different things.

    Joe, that sign you posted uses a font very similar to the one I am using on this one. I'm wondering if you used the business card trick on that or just cut as is? Also, wouldn't it be easier to just setup a second toolpath starting at a cut depth of say 0.01 instead of having to unclamp the material, slide business cards under it, and reclamp it, and hope it's in the exactlly same place? It seems duplicating a toolpath and changing the cut depth takes a couple seconds and it's done. Sometimes if I'm unsure I'll create 2-3 extra toolpaths like that in increments just so I have them ready to run if I need them.
    ShopBot Desktop 24x18
    Spindle
    VCarve Pro 8.5xx

  9. #9
    Join Date
    Oct 2009
    Location
    Elgin Illinois
    Posts
    571

    Default

    Walt, when Joe wrote: "I've even lifted one side of a panel that's cutting a bit too shallow", it made me think of a problem I am having right now myself, (covered in another thread). But simply as a note, because my table top is not as flat as it should be, that shows up in some parts of V-carvings where the lines become too thin, because the material surface is not up high enough. By measuring, I found how low one end of the plaque is compared to the end where I zeroed the bit, then I put a shim under the low end. In the area I normally work, I have to put a .030" shim under one end.

    I'm not saying that is what Joe has going on, but in my case, resorting to shims has become required to make my V-carvings not loose some of their finer lines. Chuck
    Chuck Keysor (circa 1956)
    PRT Alpha 60" x 144" (circa 2004)
    Columbo 5HP spindle
    Aspire 8.5, Rhino 5

Posting Permissions

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