How to Carve a Wooden Sign in Autodesk Fusion

The recipe in Fusion terms

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

Insert the DXF and model the board

The DXF is in millimeters with the sign’s lower-left corner at 0,0, so it lands squarely on Fusion’s origin. One sketch per layer gives you sketches named VCARVE, POCKET, and so on, which makes every selection later far easier.

1. 1

   In the Design workspace, choose Insert > Insert DXF and pick the XY plane (Z up).

2. 2

   Set the units to Millimeters and Insert Mode to One Sketch per Layer, then insert.

3. 3

   Extrude the profile in the CUTOUT sketch by your measured board thickness, downward (negative Z). Going down keeps every sketch on the top face, where the toolpaths expect them.

Make the setup

1. 4

   Switch to the Manufacture workspace and create a milling Setup.

2. 5

   Keep the model’s orientation and set the origin to Stock box point, picking the top, lower-left corner.

3. 6

   On the Stock tab, use a relative size box with zero offsets for a blank cut to size, or a fixed size box that matches a larger board, with the sign placed where it will sit on it.

Add your bits to the tool library

Fusion files a V-bit under chamfer mill. Its taper angle is measured from the center line, half the number on the package: enter 30° for a 60° V-bit or 45° for a 90°, a tip diameter of 0, and a diameter of 12.7 mm (1/2 in). Add the end mill as a flat end mill, 3.175 mm (1/8 in) or 6.35 mm (1/4 in).

V-carve the letters with 2D Engrave

Engrave sinks the V-bit as deep as each closed letter shape allows, which is the V-carving the recipe means.

A flat depth takes one more operation, because Engrave stops at its bottom height and leaves whatever’s in the middle of a bold stroke. Ahead of the Engrave, add a 2D Pocket on the same letter profiles with your end mill, down to the flat depth, with a radial Stock to Leave of the flat depth times 0.58 for a 60° bit (times 1.0 for a 90° bit). That keeps the end mill off the sloped walls, which the Engrave then cuts.

1. 7

   Create 2D > Engrave with the V-bit.

2. 8

   For geometry, select the closed profiles in the VCARVE sketch: letters, rules, and border line.

3. 9

   Automatic depth: under Heights, put the bottom deeper than the README’s deepest point. The bit’s own shape limits how deep each stroke goes.

4. 10

   Flat depth: set the bottom height to the selected contour, offset by minus the flat depth, and run it after the clearing pocket above.

Raised letters: 2D Pocket

1. 11

   Create 2D > 2D Pocket with your end mill.

2. 12

   Select the background region of the POCKET sketch, the area between the rim and the letters, plus the small regions inside letters like O and D. Fusion leaves the letters themselves as islands.

3. 13

   Set the bottom height 4.8 mm (3/16 in) below the top and turn on Multiple Depths with the stepdown your bit maker suggests for the wood.

Screw holes

Make a 2D Pocket on the two circles in the HOLES sketch with a 1/8 in end mill, with the bottom height at the model bottom minus 0.5 mm. A 1/4 in end mill can’t fit a 5 mm hole; drill those by hand with a 13/64 in bit after carving.

Bevel the edge with 2D Chamfer

Fusion’s 2D Chamfer follows model edges, so select the top edge of the board body, not the sketch. The bevel the recipe wants is 1/8 in (3.2 mm) deep.

1. 14

   Create 2D > 2D Chamfer with the V-bit.

2. 15

   Select the top outside edge of the body.

3. 16

   Set the chamfer width to 1.85 mm with a 60° bit or 3.2 mm with a 90° bit; either gives the 3.2 mm depth.

4. 17

   Add a small tip offset, around 0.5 mm, so the bit’s fragile point runs below the bevel instead of along it.

Cut it out with 2D Contour

1. 18

   Create 2D > 2D Contour with your end mill and select the bottom outside edge of the body.

2. 19

   Under Heights, put the bottom at the model bottom minus 0.5 mm so the cut just scores the spoilboard.

3. 20

   Turn on Tabs: rectangular, about 6 mm wide and 3 mm tall, placed by number (four to eight around the sign).

4. 21

   Turn on Multiple Depths so the cut steps down in several passes.

Simulate and post

1. 22

   Select the setup and Simulate with stock shown. Check that letters keep their serifs, the pocket floor is clean, and the tabs sit where you want them.

2. 23

   Order the operations as the README does: carving or pocket, holes, chamfer, then contour.

3. 24

   Use Post Process with the post for your controller (Grbl, grblHAL, or your machine maker’s). On Personal Use, select only the operations that share a bit and post them as one file, then repeat for the other bit.

4. 25

   Run the V-bit file, change bits, re-zero Z on the board top (never X or Y), and run the end mill file.

Finish the sign

Cut the tabs and sand them flush. Paint a V-carved sign into the letters over a sealed or masked face, then sand the face to clean the edges; a raised sign takes paint on the background, with the letter tops sanded bare. Give an outdoor sign an exterior-rated clear coat on every side.

Questions about Fusion

Can I sell signs I carve with Fusion Personal Use?

Personal Use is for non-commercial work, so a selling shop needs a commercial Fusion license. Our license lets you sell the signs; Autodesk’s governs the software.

Why are the air moves so slow?

Personal Use posts rapid moves at the cutting feed rate. It’s a license limit, not a fault in the file.

Engrave cuts too deep on bold letters.

Set the bottom height to the README’s flat depth and clear the floors with a 2D Pocket first, as described above.