MC Etcher Bits for CC Setup

I have both the 90 and 120 degree MC Etcher bits ordered and on the way. I watched the c3d video announcing the MC Etcher but that gave little info about usage.

Can anyone experienced with a diamond drag bit give some guidance on how they set up the tool in CC. The parameters used to set up the bit for doc, plunge and IPM.

Thanks. I want to get the bits set up in database so they are ready to use when I get them in the next few days.

Check this out for reference values:

I tend to use 0.1" DOC (the precise value should not matter much, due to the spring load), and 200ipm (because raster/hatch patterns will take a loooooong time if you go slower)

EDIT: plunge does not matter much either but “30ipm” seems to be a good safe value.


@WillAdams has a tutorial which includes the tool setup for acrylic here:

The settings he used (and I used the same in my testing) are 381mm/min (15ipm) plunge, 1143mm/min (45ipm) feedrate, and 0.5mm (0.02 in) DOC. The tool is defined with 0 RPM, but Carbide Create spits up an error when you actually try using the tool at 0 RPM, you have to change it to 1 to assign the tool to a toolpath. I used those settings on acrylic and whatever metal a Ball mason jar lid is made out of and got reasonable results.

The 90 degree MC Etcher storage tube is labeled with:
Bit number: #503E
Type: Drag bit
LOC: .0625"
Diameter: .250"
Angle: 90
OAL: 2.43"


So I created a library and partially populated it. Please comment on any fields that need values. Should the type be Vee?

number vendor model URL name type diameter cornerradius flutelength shaftdiameter angle numflutes stickout coating metric notes machine material plungerate feedrate rpm depth cutpower finishallowance 3dstepover 3dfeedrate 3drpm
503 Carbide3d 90 Dia Drag MC Etcher - Diamond Drag Bit – Carbide 3D 90D Diamond Drag Dia Drag 0.25 0.25 90 0 Shapeoko Brass 15 45 1 0.02

How did you use it to make a tool path. Did you do a VCarve, technically the bit is a Vee Bit. Would someone please post a CC file with the 90 and/or 120 Diamond Drag so I can see what you did.

In my opinion you should not declare is as a V, rather as a (very) small diameter square or ball.
And then only use contour/profile toolpath (or texture toolpath), because using a v-carving toolpath will probable not result in what you want.
99% of the time, a profile toolpath “on” a selected vector, with 0.1" depth of cut (single pass) will be the best option for tracing outlines, and a pocket (same DOC, very small stepover) can be used to fill areas


I have the MC Etcher set up as a engraver in CC, not a vee bit. I think of the bit as a pencil more then a end mill. You probably don’t want the 0.25" you have set up as the cutting diameter, that will make pocket operations (to fill an area) difficult. I have the cutting diameter configured as .004" (.1 mm), based on Will’s tutorial.

Attached are a couple of my test files. “Etcher Test.c2d” was on acrylic using a no-offset contour path. You can see the results here:

“Texture Test.c2d” was on a granite tile from Lowe’s:

The heart/paw was filled with a .02" stepover texture in Carbide Create, the label (the name of one of our cats that passed away) is filled as a .008" stepover pocket operation. Everything also gets an outline using a no-offset contour for a well defined edge. I did the outline first because I am impatient and like to see what the design will look like:

Doing the outline first might also keep any chipping contained inside the outline (but that is just a guess, I am new to this stuff).

Etcher Test.c2d (50.1 KB)
Texture (197.6 KB)


Thanks so much for your advise. I will read and reread a few times to adsorb. I downloaded the 524 CC Beta in hopes it would have the 503 and 504 bits in the library but there are not there yet.

This is what I like about this community, helping others.

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