First time with diamond drag bit

Do you have to use Vcarve or Aspire for this or could it be done in CC?

Also, which particular bits work? I am interested in trying it, but would like to keep startup costs low (below $50?)

I am using Vectric V-Carve desktop, but I am sure there are other programs to generate the different paths for diamond drag engraving (DDE).

I do not use CC, so I cannot comment on it. I started using Inkscape and Makercam since everything I am doing is 2D, and now I am so comfortable with that process, I am hesitant to find something new.

With V-Carve, I still do all my 2D design in Inkscape, and then import the SVG file into V-Carve to generate the tool paths.

I figure one day I will learn how to use V-Carve properly and fully, but that day is not today.

Regarding the DDE bit, I believe the one from is the least expensive one I have seen online. The WidgetWorks one is 3x as much. I have the one from benchtopprecision and I really like it.

1 Like

I have done it in CC. Certainly a little easier in VCarve, but CC will do it too. Here’s a flag I did:

You basically treat it as a very small end mill. Settings are posted in that post. My drag bit was $50 off eBay.



Good Evening @madhatter what program do you use to generate your toolpath? if it is Fusion360 would you mind sharing the file?

Love your work !

speak soon i am sure

1 Like

I use Inkscape to turn the logos into vector files, then I use Vectric V-Carve (Desktop) for creating the G-code.

EDIT: Also, is kaput! Homann Designs has the same diamond drag engraver though.


Well, I ordered a diamond drag bit, and I picked up some black granite floor tiles yesterday. All I have left is figuring out what on earth I’m doing, eh? :laughing:

I’ve got my artwork into a nice SVG, as I’m doing a laser engrave on some bamboo cutting boards. I did all the toolpath work on that in LightBurn, which makes it really easy to define fills (line or crosshatch). Now, I just have to do the analogous thing for a diamond drag bit. Carbide Create doesn’t let you define fills like that, so it’s out. Vectric V-Carve would send the project way over budget. It’s possible to bodge virtually anything with enough work in Fusion 360, but that doesn’t seem the most effective approach (and I don’t have enough time left before Sunday).

So, looks like my options are either settle for whatever fill I can get out of Carbide Create (although it will not please my artistic sensibilities) or splurge on V-Carve (although it will not please my budget)… or…

If I use LightBurn to generate “laser” G-code (no overscan, 2D), then convert the “dark” (S0) moves to “raise the spindle, move, lower the spindle”, that seems like it should get me just what I’m looking for. I’ll just have to run one little regex (match: “^G1(.*)S0$”, replace with: “G0Z5\r\nG0\1\r\nG1Z-5F750”) and do a quick hand edit of the beginning and end of the file to get things ready.

Well, tonight’s laserin’ time, but I think I’ve got a plan that may be up to scratch for diamond drag bit engraving. (Looking through threads, it looks like starting numbers that should work are around ~2.5mm spring compression, 750mm/min plunge, 2500mm/min feed, and a spritz of water.)

On further review, two regex replacements (and then fix just the header):

  • Search: ^G0(.*)$
    Replace: G0Z5\r\nG0\1\r\nG1Z-5F750
  • Search: ^G1(.*)S0$
    Replace: G0Z5\r\nG0\1\r\nG1Z-5F750
1 Like

@ClayJar Have you played at all with Carbide Create’s texture tool paths? I think they will do what you are looking for.

1 Like

The Carbide Create texture toolpaths are as close as Carbide Create can get to what I want, but they don’t quite get there. They do let you set an angle, and you can get the right depth. They don’t let you do a uniform fill that covers 100% of the shape. I imagine you can probably get acceptable results from them, but you can’t quite get all the way.

I imagine many people would be quite happy with the results, but since I’m completely at home throwing regular expressions around to munge exactly what I want into G-code… (Programmers have the strangest concepts on “fun”, eh?)


I think you are on it with just replacing the laser on / laser off with Z-Down and Z-Up. You’ll lose the ability to change the line thickness (from the variable laser power) but with as many hatching and cross-hatching combinations, you’ll still be able to get a lot of different fill densities and patterns.

Can’t wait to see how things turn out.

I did it in CC by creating a tool with a small tip, then cutting filled areas as pockets. It’s not super artsy, but it works. VCarve will definitely do it with a “quick engrave” tool path, and what you’re doing with Lightburn sounds like it’ll work too (just a little more handiwork and a lot less cost). Pretty cool stuff!!!


1 Like

I was working on a reply in another thread, and in looking deeper into the “Texture” toolpath option in Carbide Create, I ended up running some experiments and examining the resulting G-code. Looking at the results of one of the experiments, it became clear what the “Min Depth” and “Max Depth” values in the “Texture” toolpath options actually mean. They’re the range of the maximum depth of each texture segment, not the actual minimum and maximum depths. Each texture segment’s actual Z depths range from the surface at the ends to a randomly selected maximum depth somewhere between the entered “Min Depth” and “Max Depth” values.

So, “Texture” toolpath option does not yield G-code suitable for diamond drag bit engraving.

1 Like

Interesting… I would have thought setting “Min Depth” and “Max Depth” to the same value would have yielded a single consistent depth per pass. Is that not the case?


It is not. Here’s a quick annotated screen crop of a few texture toolpath segments viewed from the side (i.e. an edge view through invisible stock).


In this example, I’m just showing the first few toolpath lines starting from a very small part of the design, as otherwise the view would just be a solid mass of overlapping lines. If you were looking straight down along the Z axis, each blue curve in the illustration would be one straight line. Looking edge-on (parallel to the wasteboard), you can clearly see that each blue curve starts basically at the surface, curves down to some maximum depth, and curves back up to the surface.

The “Min Depth” and “Max Depth” settings in the “Texture” toolpath options set the bounds for randomly selecting each individual texture toolpath segment’s maximum depth. So, the actual minimum depth for each segment is the top, i.e. “Start Depth”, and the actual maximum depth is some randomly selected value between “Min Depth” and “Max Depth”.


How long should a diamond drag bit last? The $50 any better than the $200 ones?

1 Like

I don’t know about $200 drag bits but I purchased a set with 3 different angle bits with a spring holder on E-Bay at less than $50 a few months ago and I have done several carves in granite and aluminum and I have used only one in the set but it is as sharp as it was at the beginning. I don’t know how much you will use but unless you go into a large production, save your money, you can buy 3 other sets for the price of the expensive one.


Do you have a link for the one you bought?

I bought mine from this store but looking at the invoice, it was $50 for the bit and holder and another $50 for the replacement bit and extra spring.

1 Like

Just keep in mind that diamond tipped bits are very strong but brittle. So ease into the cuts. Diamond tips can be dislodged if it is used too violently. I use a diamond topped tool from Oneway to dress my wheels on my slow speed grinder. So even though the diamond is the hardest thing in your shop it can be damaged if you do not be very gentle with it. Remember that although the diamond is hard it is anchored with material that is less hard than the diamond and the diamond top can be broken off even by dropping the bit.

I bought a drag bit, and now I am trying to figure out how to make a tool path in Fusion 360. It works if I use 2d Trace. But I can’t find any solution to using it in Parallel. When I used the drag bit, I got an error: “Invalid tool type for milling.” That’s logical because it’s an engraving bit.
So, any advice from more experienced users? Do you just use a different “fake” tool just to do the trick in Fusion, and for machining, you use drag bit? Thanks

Yeah, I remember hitting that specific road bump and I created a fake tool

1 Like