Carving small letters

There were some notes at:

  • V-cutting — special purpose, used for engraving or chamfering, or cutting parts w/ angled sides. Identified by the angle of the V — 90 degree bits can be used for mitering. Sharper angles will cut deeper for a given width of cut. Engraving bits with a single-flute (look like half cones) are able to cut more deeply w/ a single pass.[19] Most V-bits are unable to clear chips, so require slower speeds.[20] See also V-carving reference books.
    • If work cannot be completed in a single pass, some operators will grind the tip to a 0.5–1mm radius ball point so as to minimize stepping (esp. when cutting wood). Discussion here: Steps in V carve file
    • number of Passes — Size guidelines for adding a radius at the tip (may vary based on bit angle and material):
      • <10mm — one pass
      • 10–20mm — ~0.5mm
      • 20–35mm — ~0.75mm
      • > 35mm — 1mm radius
    • The tradeoff is feature size vs. feature depth — an acute angle allows one to cut a smaller, finer feature w/ more depth, while a more obtuse angle allows one to cut a larger area w/ a single pass and while having a single bottom, as opposed to a ragged set of scallops.
      • Recommended bit angle for a given text size:
        • <1" 45–60°
        • 1–2" 60°
        • 2–4" 60–90°
        • 4–6" 90°
        • 6–10" 90 to 120°
        • > 10" 120° or greater
    • Material guidelines:
      • hardest timber available
      • use conservative plunge and feedrates even when doing more than one pass
      • avoid overlapping V-cuts — tends to cause splintering at the top edge, leave a ~0.5–1mm gap at the top
      • use a cutter w/ centered/symmetrical geometry
    • Formula for calculating the effective diameter of a V-bit at a given depth in Excel this is:[21]

=TAN(RADIANS(B3)) * B4 * 2

Where B3 is the angle in degrees and B4 is the depth in inches

Site to calculate offsets/depths: Angular Size Calculator [22]

Excellent image noting width considerations: Carve letters depth - #5 by JaredHooper

Note that the angle of a given endmill may vary slightly, esp. if it has been resharpened. One suggested technique is to prepare a series of files set to V-bits at different angles and cut them in a piece of scrap so as to determine which angle best suits a given endmill.[23] Images along with a link to a Vectric post: CNCnutz: Test your V-bit angle - episode 151

A further consideration is that SFM will vary based on how far up or down the taper a given section of cut is occurring at:

1 Like