My board is bigger than 24 in. Can VCarve Desktop handle it?

Desktop’s job size stops at 24 x 24 in. Use VCarve Pro, or tile the toolpaths, which means sliding the board partway through.

Do I need to explode or weld anything?

No. The letters are already closed outlines, with no text objects or open vectors, so they’re ready for toolpaths.

Can I reuse the toolpaths on my next sign?

In VCarve Pro, save a toolpath template once and apply it after importing the next DXF. The layer names never change.

How to Carve a Wooden Sign in Vectric VCarve

Vectric VCarve was made for exactly this kind of job, and the DXF’s layers come straight into its layer list, so most steps are one right-click and one toolpath. This guide follows VCarve 12.5; Aspire has the same toolpaths in the same places.

Desktop or Pro? Both have every toolpath used here. VCarve Desktop caps a job at 24 x 24 in, so a 36 in sign needs Pro or tiling. Pro adds toolpath templates, which let you save this setup once and reuse it on the next sign.

Updated October 3, 2026.

The recipe in VCarve terms

Your README lists only the steps your sign needs, in this order. Here's what each layer becomes in VCarve:

Layer	Bit	In VCarve
VCARVEV-carved letters and border	V-bit	VCarve toolpath (V-Carve / Engrave). For a flat depth, tick Flat Depth and add the end mill under Use Clearance Tools.
POCKETBackground around raised letters	End mill	Pocket toolpath on the whole `POCKET` layer.
HOLESScrew holes	End mill	Profile toolpath, Inside, through the board.
CHAMFERBeveled edge	V-bit	Profile, On the vector with the V-bit, or the Chamfer toolpath.
CUTOUTCut the sign out	End mill	Profile toolpath, Outside, with Add tabs to toolpath.

Set up the job

1
Create a new file and choose Single Sided.
2
Enter the board width and height from the README, or the larger blank’s, and your measured thickness. Inches are fine; the import converts.
3
Set Z Zero to the material surface and the XY Datum to the lower-left corner.

Import the vectors

VCarve reads the DXF at the size it was drawn and keeps its layers, so VCARVE, CHAMFER, CUTOUT, and the rest show up in the layer list. VCarve can import SVG as well, but stick with the DXF here: the layers come with it.

4
Use Import Vectors (with the File menu’s import options) and pick the .dxf.
5
Compare the sign’s size with the README.
6
Select everything and position it so its lower-left corner sits at X 0, Y 0, or about 1 in in from each edge on a larger board.

V-carve the letters

Right-click the VCARVE layer and select all of its vectors: letters, rules, and border line.

7
Open the VCarve toolpath and pick your 60° or 90° V-bit.
8
Automatic depth: leave Flat Depth unticked so the bit goes only as deep as each stroke needs.
9
Flat depth: tick Flat Depth, type the README’s value, and under Use Clearance Tools add your end mill to clear the flat floors.
10
Calculate, and look over the preview for any stroke VCarve flags as too narrow.

Raised letters: Pocket

Select every vector on the POCKET layer: the rim’s inner edge, each letter, and the counters inside letters. VCarve treats the nested shapes as islands, so the letters keep their full height.

11
Open the Pocket toolpath with your end mill.
12
Set Cut Depth to 3/16 in (4.8 mm), or the depth in your README.
13
Offset clearing leaves the cleanest floor around letters; raster is quicker across a big open background.

Screw holes

Select the two circles on the HOLES layer and make a Profile toolpath, Inside, at the README’s through depth with a 1/8 in end mill. A 1/4 in end mill is wider than the 5 mm holes and VCarve won’t cut them; drill them by hand at the marks instead. The Drilling toolpath only plunges at each circle’s center, so it suits a drill bit, not these holes.

Bevel the edge

The recipe’s bevel is the V-bit run right on the outline, 1/8 in (3.2 mm) deep. The simplest route is a Profile toolpath, On the vector, with the V-bit and a cut depth of 1/8 in. VCarve’s Chamfer toolpath works too: give it the same depth and pick the side that puts the slope on the sign, which the preview shows plainly.

Run it before the cutout, while the sign is still part of the board.

Cut it out with tabs

14
Select the outline on the CUTOUT layer.
15
Make a Profile toolpath, Outside, with your end mill and the README’s through depth.
16
Tick Add tabs to toolpath and edit the tabs: about 1/4 in long and 1/8 in thick, four on a small sign and more on a long one. Triangular 3D tabs are easier to clean up.

Preview and save the toolpaths

17
Preview all the toolpaths with the material shown and look the sign over, then reset and check each toolpath alone.
18
Open Save Toolpaths and choose your machine’s post processor.
19
Save one file per bit, in the README’s order. Only a post for an automatic tool changer can put different bits in one file.
20
At the machine, zero X and Y on the lower-left corner and Z on the board top, run the V-bit file, then change bits and re-zero Z only.

Finish the sign

Saw through the tabs and sand them. For painted letters, seal the face before carving (or use masking film), paint into the carving, then sand the face back once dry. On raised signs, paint the background and sand the letter tops. A sign that lives outside needs an exterior clear coat on all sides so it doesn’t cup.

Questions about VCarve

My board is bigger than 24 in. Can VCarve Desktop handle it?: Desktop’s job size stops at 24 x 24 in. Use VCarve Pro, or tile the toolpaths, which means sliding the board partway through.
Do I need to explode or weld anything?: No. The letters are already closed outlines, with no text objects or open vectors, so they’re ready for toolpaths.
Can I reuse the toolpaths on my next sign?: In VCarve Pro, save a toolpath template once and apply it after importing the next DXF. The layer names never change.