How to carve small text on plastic?

Hi all,
I am trying to make placards in 2 and 3 colour, layered vinyl (Edit…Rowmark acrylic) and i’m having some trouble finding the correct way to do this. They are small so text size is around 3-4mm high.

There is the contour cut option using a 0.2mm end mill which would take an enormous amount of time due to the slow feed and, there is the V-carve option which seems like it won’t give a clean finish when cutting through multilayered material. Not to mention i’m finding it impossible to work out how to get text to be a single path to generate a neat toolpath.

Do I need a certain software to do this?

Hi @Aero3D,

Maybe worth a try though, with a good quality 30° Vbit ?
What stock thickness are we talking about ?
Here’s an example of using a 60° Vbit on two-layer HDPE, not quite relevant because it was with much larger letters, but there is no reason why it could not work using small letters and a 30° vbit.

About the neat toolpaths: can you post an example of a design file with toolpaths that are not as you would like them to be ? Sometimes the way you select different parts of the text to create toolpaths has a lot of impact on the resulting toolpath. Beyond a certain point, if you do a lot of vcarving you may want to look at other specialized software like Vectric VCarve, which tends to generate more optimized v-carving toolpaths (but it comes at a cost)


I’m using 1.4 - 1.6mm stock so depth of cut is half that.

If you select text in CC and change height to 4mm, you’ll see the lines are quite ragged looking. Is this how it will present once cut?
I guess i’ll buy a couple of vee bits and give it a try. I also don’t mind buying whatever software I need to get the job done but I’d like to know how the job is done and then get the correct equipment.

1 Like

The preview in CC has a limited resolution, so at small sizes like that it will have artefacts that would not be there in the actual cut.

That said, carving 3-4mm high letters 0.7mm deep on a Shapeoko will require a properly tuned machine and appropriate feeds & speeds. If you can post here an example .c2d file of what you want to cut, it will help people here provide specific recommendation for your usecase.

However you mentioned vinyl in your first post, which I associate to very thin material and using a drag-knife for cutouts (or using a dedicated machine like a Cricut), but then you mention 1.6mm stock so it must be something else. Would you have a link/example/picture for the stock material you plan on using ?


Oh dear, I did mention vinyl. I guess that indicated my state of mind when looking for help. :worried:
I’m using Rowmark acrylic sheets which come in a variety of colours and sizes but the thinnest I’ll be dealing with is 1.3mm.

That is good to know about the preview in CC and gives me some much needed hope.

Thank you so much for your help Julien.


You may be interested in that thread then, where we experimented a little around vcarving acrylic sheets:

I have some colored acrylic sheets left so if you want me to run a test cut I’ll be happy to try a few recipes/tools for you.


I will take a look at that thread.

I’ll also order some vee bits as they seem to be the tool I need.
What size/angle do you think I should try? The smallest text height in CC would be 3.6mm.
I can send a file when I’m at work tomorrow but I’m just using Arial at 3.6mm in a 19x14 border.
Examples of text will be;



1 Like

The shapeoko wiki has a section about this, which mentions “45-60°” for letters below 1", but yours are much smaller than 1", so I have a feeling that it may be difficult to pull off using a 60° vbit. My bet would be to use a 30° vbit and limit cutting depth to half the stock thickness using an Advanced v-carve toolpath in Carbide Create.

I don’t carve text much, but I know some folks here have v-carved small text when making custom front plates for their projects, they may be able to provide better insights.

I have some new 30° vbits I have been wanting to use for a while, so I’ll try and test something later today.
Regardless, getting one 60° and one 30° vbit will not go to waste if you’re going to do a lot of text carving.


Yeah, for smaller text, look into 30 degree endmills — I’d be glad of a guidance on what size one should start considering such small endmills — my estimate would be ~1/4" (~6–7mm) or less.


I use .25” 30 degree single flute on all of my acrylics. Varying tip diameters, but this makes little difference. Say .01 or .001, visually, at the depth generally used for text, not much to see. I don’t use vcarve paths, just trace.


I still have some scraps from the adventure in plastic carving Julien already posted, so I can help with experiments as well. I also have a 15 degree vbit that I need to try in acrylic but haven’t gotten around to. It work quite well in wood in my limited usage so far.


The key to small fonts is “straight line” fonts. I’ve used that along with a 30 degree engraving bit in less than ⅛” text with success.


Unfortunately, the number of single line fonts is quite limited — there are the Hershey fonts, some specialty fonts associated w/ CAM or G-Code programs, and that’s about it.

There is a commercial product as well — one of their products simulates single line fonts with an incredibly narrow font, so the paths are doubled when cutting, but the approximation of a single font is quite good.



1 Like

The OP’s app sounds like a commercial faceplate or similar. Its possible that just plain text would be adequate, as opposed to needing script or delicate fonts as a sign might need.

(Oh well, just thought I’d reply since all we’re doing is waiting for a hurricane to blow everything we own into a pile of wood carving supplies. Or not! :slight_smile: Sorry for the hijack.)


Tks Julien, I have ordered various V bits so I will have another look at this when they arrive.

Forgive my ignorance. but what is trace and how do I do that?

How can I know if a font is a ‘straight line’ font?

Hey Cam,

VCarve programs use varying cutter depths to produce detail between vectors. A trace follows a vector line at a prescribed depth. a Vcarve path will have a relatively square corner when designed as such. The trace will have a radius equal to the cutter at x depth. I use single line fonts, which for descriptive purposes can be imagined as a single open vector. Think hand written letters.

Your typical digital font can be imagined as outline of that single line, a closed vector. A simplification, as single line fonts are not necessarily an open vector, but I think that should give you a good idea of the difference.

Using something like fusion, I place single line fonts in a sketch. These are never extruded. In CAM, I select these open sketch vectors and run a trace. The trace follows the line at whatever offset I determine.


I believe “straight line” was meant to be “single line” — please see the links I posted above.

@WillAdams is exactly correct and sorry I wasn’t more succinct about straight line vs single line fonts. I find many more straight line fonts like this one: image

What I’ve done with one like this one is create a very small inward offset (after converting to vectors) that will be treated like a single line font. I use Vectric Vcarve software that has several ways to do this.

1 Like