How to Carve a Wooden Sign in Estlcam

The recipe in Estlcam terms

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

Open the drawing and set the zero

Estlcam opens DXF and SVG files directly. The DXF is in millimeters; Estlcam works in mm by default, so the sign comes in at its real size.

1. 1

   Open the .dxf with File > Open and compare its size with the README.

2. 2

   Use the Zero tool to put the zero point on the sign’s lower-left corner.

3. 3

   Add your bits to the tool list: the V-bit with its angle (60° or 90°) and the end mill with its diameter, plus feeds and speeds from your bit maker.

V-carve the letters with Carve

Estlcam’s Carve path is its V-carving mode. It needs a pointed bit, and it can hand the wide floors to a second, flat tool.

1. 4

   Choose Carve, pick the V-bit, and click the letters, rules, and border line from the VCARVE layer.

2. 5

   Automatic depth: leave the depth limit off, so the bit follows each stroke.

3. 6

   Flat depth: set the depth limit to the README’s value and choose your end mill as the pocketing tool. Estlcam then clears the flat floors with the end mill and cuts the walls with the V-bit.

Raised letters: parts with an island hole

Estlcam builds the background pocket from two kinds of path. The letters are marked as parts (shapes to keep), and the rim’s inner edge is marked as a hole that clears everything except those parts. Order matters: mark the letters first.

1. 7

   Choose Part and click each letter outline on the POCKET layer, giving them the pocket depth of 3/16 in (4.8 mm).

2. 8

   Mark the centers of letters like O and A as Hole paths with pocket clearing, at the same depth.

3. 9

   Choose Hole, click the rim’s inner outline, and turn on island clearing, so Estlcam clears around the letters down to 3/16 in.

Screw holes

Mark each HOLES circle as a Hole path with the 1/8 in end mill, at the README’s through depth. A 1/4 in end mill can’t fit the 5 mm holes; drill them by hand afterward.

Bevel the edge

Choose Engraving, centered on the line, pick the V-bit, and click the sign’s outline at a depth of 1/8 in (3.2 mm). This runs before the cutout, while the sign is still part of the board.

Cut it out with tabs

1. 10

   Choose Part, pick the end mill, and click the CUTOUT outline (the one under the bevel line; they’re the same shape).

2. 11

   Set the depth to the README’s through depth.

3. 12

   Add tabs by clicking on the outline: four or more, about 1/4 in long and 1/8 in high.

Save the CNC program

Estlcam asks for any depth you haven’t set when you save. Use the README’s numbers, and check the 3D preview before you leave.

1. 13

   Put the paths in the README’s order: carving or pocket, holes, bevel, cutout.

2. 14

   Use Save CNC Program. If your controller can’t pause for a tool change, save one program for the V-bit paths and another for the end mill.

3. 15

   Running an Estlcam controller board? Start the job from Estlcam itself, with zero on the lower-left corner and Z on the board top.

4. 16

   Change bits between programs and re-zero Z only.

Finish the sign

Cut the tabs and sand them away. For painted V-carved letters, seal or mask the face before carving, paint, then sand the face clean. Raised letters pop with a painted background and bare, sanded tops. Outdoors, coat every face with an exterior clear finish.

Questions about Estlcam

Is the free version enough for a sign?

It does everything here; it just gets slower to open and save files the more you use it, until you buy a license.

Estlcam cut around my letters instead of clearing the background.

The rim was marked before the letters. Mark the letters as parts first, then the rim as a hole with island clearing.