I’m currently using a 20 degree, single flute carbide tip, but I’m open to advice. With VCarve Desktop, I tried a vcarve toolpath which works great on wood but it goes way to deep and therefore won’t work on metal. Also, the repeated passes mar the metal quite a bit. I then added a small (0.3mm) Flat Depth amount but that gave the engraved text a flat bottom, not what I’m after. I then tried a profile toolpath, but you can either engrave outside, inside or on the path but not “between” if that makes sense.
From my understanding, a single line font could work but I don’t know how to create a single line font
from a specific True Font, in this case Bookman Old Style.
Could anyone suggest how I can achieve the result I’m after?
I had good luck w/ a V endmill in brass using Vectric VCarve:
but was cutting around the text, rather than directly incising the text — doing that is challenging since the tip of the V has a very low effect speed — if memory serves I was ramping in and had to carefully balance the plunge rate even then.
For the V endmill surface speed thing — consider a V endmill which has a circumference of 1" at the top — if the tool is turning at 10,000 RPM then the effective surface speed at the top is 10,000 inches per minute — if you move down the V to where the circumference is 0.5" it is only 5,000 inches per minute — this continues until one reaches the tip, where despite turning, the effective surface speed is 0 since the center of the tip just stays in place. This is part of why engraving tools for metals have rounded tips.
Unfortunately, there isn’t really a way to make an outline font into a single line font — that’s the advantage of V carving that it carves down the centerline and optimally captures all the detail at the surface.
I believe that it would be worth experimenting w/ ramping/leading in, and plunge rate — hopefully you’ll find a feed and speed setting which works for you and the material you are cutting.
There is a video on line of relief engraving in brass. The final pass was with a 20 degree v bit , 0.2mm ( I assume this was the tip diameter?), 24500 RPM, 1600 mm/min, 0.05 mm depth of cut. I wonder if a v carve tool path limited to this depth of cut for each pass would be successful?
+1 for that. I just did some lettering on Sterling silver for a present and the diamond drag engraver gave a great look. I guess if you wanted to inlay the silver with something you may still need to fully machine out.
Diamond drag engraving will not go very deep. perhaps 0.1-0.2mm max. But it will look very crisp. For very small but deep letters, I would try something like a PCB engraver (501/502), which should cut cleaner than a woodworking v-bit. The more tapered they are, the more fragile they are. I run the 502 about 25% slower than the 501. The 501 I would probably start with 24000 RPM, 200-250 mm per minute, 0.08 mm depth of cut. You may be able to get away with slightly more aggressive settings in sterling silver but it will take experimentation.
@wmoy - Winston your videos are just brilliant! Thank you for your response. Yes I’m experimenting now with various V bits and am probably going to get the Diamond drag bit to see what I can manage with it.