How to Carve a Wooden Sign in Carbide Create

The recipe in Carbide Create terms

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

Before you start

Unzip the download and keep README.txt open beside Carbide Create: it has your board size, the depths, and the steps your sign needs. Measure the board’s real thickness with calipers, since a “3/4 in” board is often nearer 0.72 in.

Carbide 3D sells the bits the recipe calls for, and they’re already in the tool library: #302 is the 60° V-bit and #301 the 90°, both 1/2 in across, while #102 and #201 are the 1/8 in and 1/4 in flat end mills. Another brand? Add it with its true angle and diameter so the V-carve depths come out right.

Painting a V-carved sign? Seal the face with shellac or a clear coat, or lay masking film over it, before it goes on the machine. That stops paint wicking into the grain around the letters.

Set up the job

Carbide Create reads a DXF’s numbers in the job’s units, and the sign files are in millimeters. Set the job to mm while you import; you can switch back to inches afterward and everything converts.

1. 1

   Start a new design and open Job Setup.

2. 2

   Set the units to mm for now.

3. 3

   Enter the board width and height from the README, or those of the bigger blank you’re cutting it from, plus your measured thickness.

4. 4

   Set the zero position to Lower Left and Z zero to the top of the stock.

Import the drawing

The shapes usually land on one layer, which is fine: you pick them by clicking. The CHAMFER and CUTOUT outlines are the same shape stacked twice, so either copy serves both toolpaths.

1. 5

   On the Design tab, use Import and choose the .dxf from your download.

2. 6

   Select everything and compare its width and height with the README. If it’s 25.4 times too big or too small, undo, fix the job units, and import again.

3. 7

   Move the drawing so its lower-left corner sits on the stock’s lower-left corner. On a larger board, set it about 1 in (25 mm) in from each edge to leave room for clamps.

4. 8

   Switch Job Setup back to inches now if you’d rather work in them.

V-carve the letters (VCARVE)

The VCARVE layer holds the letters, any rules beside the words, and the border line if you chose one. They all carve in one toolpath.

1. 9

   Drag a selection box just inside the sign’s outline to catch the letters and border. Shift-click the screw-hole circles, if there are any, to drop them.

2. 10

   On the Toolpaths tab, choose V-Carve and pick your V-bit.

3. 11

   If the README’s depth says automatic, leave the maximum depth unset (or deeper than the deepest point the README gives) so the bit follows each stroke.

4. 12

   If it gives a flat depth, enter that as the maximum depth and turn on clearing with a pocket tool, choosing your end mill. Carbide Create then makes two linked toolpaths: the end mill flattens the wide floors and the V-bit cuts the sloped walls.

Raised letters: clear the background (POCKET)

On a raised sign, the POCKET layer is the inside edge of the rim plus every letter outline. Pocket them together and Carbide Create keeps the letters, and the centers of letters like O and A, standing as islands.

1. 13

   Select the rim’s inner outline and all of the letter outlines.

2. 14

   Make a Pocket toolpath with your end mill, 3/16 in (4.8 mm) deep, or the depth in your README.

3. 15

   Look at the 3D view: the letters should stand proud with nothing left in the background.

Screw holes (HOLES)

The two holes are 5 mm (a hair over 3/16 in), sized for #8 screws. With a 1/8 in end mill, select both circles and make a Pocket toolpath to the README’s through depth, which is the board thickness plus 0.5 mm, so it just scores the spoilboard.

A 1/4 in end mill is wider than the holes, so Carbide Create can’t fit a toolpath inside them. Skip the step and drill them by hand at the marks with a 13/64 in or 3/16 in bit, or swap to a 1/8 in end mill for this one toolpath.

Bevel the edge (CHAMFER)

Carbide Create has no separate chamfer toolpath; a contour run right on the line with a V-bit does the same job. Run it before the cutout, while the board is still held all the way around.

1. 16

   Select the sign’s outline.

2. 17

   Make a Contour toolpath with the offset set to No Offset.

3. 18

   Pick the V-bit and set the depth to 1/8 in (3.2 mm).

Cut it out with tabs (CUTOUT)

Since V7, tabs are placed on the shape on the Design tab, then switched on in the contour toolpath. Bought a rectangular sign and your board is already cut to that size? You can skip the cutout.

1. 19

   Select the outline and use the tab tool to place tabs: four on a small sign, six to eight on a long one, spaced evenly and off the tight curves.

2. 20

   Make a Contour toolpath, offset Outside/Right, with your end mill.

3. 21

   Set the depth to the README’s through depth and turn tabs on. A tab about 1/4 in wide and 1/8 in thick holds well.

Simulate, save, and carve

Toolpaths run from the top of the list down, so order them the way the README does: carving or pocket, holes, bevel, cutout. Drag them to reorder.

1. 22

   Click Show Simulation and watch the whole job. Look for letters missing detail, ridges left in a pocket, or tabs sitting on a curve.

2. 23

   Save the project. In Carbide Motion, load the .c2d, zero X and Y on the board’s lower-left corner and Z on its top.

3. 24

   Unsure about anything? Run an air pass first: zero Z an inch above the board and watch the machine trace the sign.

4. 25

   At each tool change, Carbide Motion asks for the next bit. A BitSetter measures it for you; without one, re-zero Z on the board top. Never re-zero X or Y mid-job.

Finish the sign

Saw or chisel through the tabs and sand them flush. For a V-carved sign, brush or spray paint into the letters, let it dry fully, then sand the face (or peel the film) until the edges are crisp. For a raised sign, paint the background if you like and sand the letter tops back to bare wood. A sign that will hang outdoors needs an exterior-rated clear finish on every face, back included.

Questions about Carbide Create

Do I need Carbide Create Pro for a sign?

No. V-carving with a flat floor, pockets, contours, and tabs are all in the free edition. Pro matters only if you want a G-code file for a machine that isn’t from Carbide 3D.

Why is there no toolpath for my screw holes?

The holes are 5 mm across and a 1/4 in end mill is 6.35 mm. Use a 1/8 in end mill for that step, or drill the holes by hand after carving.

Why does my V-carve preview go so deep?

A V-bit sinks deeper wherever a stroke is wider. If the README gives a flat depth, enter it as the maximum depth and add the end mill as the clearing tool.