V carve tool selection and settings

When using v carve in carbide create what is the best v groove tool? Diameter? Degree? Also what text works best for signs?

Last question, do you set your depth or go off default settings?

Having a tough time learning v carve! Thanks in advance!!

We have a bit about this here:

https://my.carbide3d.com/gswso/12

https://my.carbide3d.com/gswcc/08

There’s a bit about angle and how it relates to font/feature size 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.
    • 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

    • the # 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:

      =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

This thread discusses it as well

and has an image which shows width considerations

Like anything else, start with the feeds and speeds in Carbide Create as a conservative guideline and use a technique such as: Calibrating Feeds and Speeds When Using Carbide Microtools to work up optimal settings for your endmill, machine, and material.

The elephant in the room is that Carbide Create doesn’t account for an inability to carve wider than the endmill diameter, so a too large square will become a four pointed star — you can work around that by insetting the geometry twice, and carving as a V carve using the inner and outer geometry, and cutting the in-between as a pocket at the depth which the V carve will reach.

I have had best results when v carving fonts and images with a 45deg bit, I use it for almost everything.

Because the diameter of the tip of the v bit is so small, the cutting speed is very low, so I run mine at max rpm (24k rpm) and about 80ipm usually yields quite good results for me.

Good general rule of thumb is that bigger angled v bits (i.e 90deg) are better for jobs with less detail, and for finer or more detailed work a lower angled bit (i.e 30deg) will give better results

1 Like

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.