I’m trying to engrave text into metal (sterling silver) and have not been successful. The sample image illustrates what I’d like to achieve but my text is smaller in height (4mm).
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.
Do you know what hardness your silver is?
Silver is a soft metal so the harder temper you start with I would expept best (but not good) results.
Due to the low surface speed of the tip of any V-cutter you want maximum RPM (24k on a Nomad3 helps) @wmoy did a good video, see here: https://youtu.be/QuM6Ic1Cxok?t=223
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.
Gunter
