CNC + Laser: Engraving 3D Plaques

Some of the best wood plaques aren't made on a single machine, they're a CNC + laser handoff. The CNC carves the 3D profile (raised border, beveled edge, recessed center, contoured surface). Then the part moves to the CO2 laser to add the engraved details: names, dates, scripture, fine artwork. The hard part isn't either machine, it's getting the engraved details to land EXACTLY where the CNC carved features are.

1 · Creating vectors in the software 2 · Just off the CNC 3 · On the CO2 4 · Complete Click a thumbnail to view full size

Why CNC + laser instead of one machine

• CNC owns 3D geometry: pockets, bevels, V-carved borders, contoured surfaces. A laser can't push wood off in millimeters per second the way a router bit can.
• Laser owns fine detail: text under 6mm tall, photo engraves, scrollwork, hairlines. CNC can do small text but burns through bit life and doesn't match laser sharpness.
• The combo: a plaque with a beautifully carved 3D border AND a crisp portrait or fine-text inscription in the center. Neither machine alone gets you there.

The alignment problem

When the plaque comes off the CNC, it doesn't have a "home" in your laser bed. You need to register the part so the engraving lands within ±0.2mm of the CNC features. Two reliable methods.

Method 1: Tool Layers (T1 / T2) inside Lightburn

Lightburn's Tool Layers are special layers that show on screen and frame with the red dot, but DO NOT output during the run. They're for alignment only.

1. Build one master Lightburn file with both the CNC profile geometry AND the engrave detail in the same project, perfectly registered to each other on screen.
2. Convert the CNC features to T1 (right-click layer → set layer to T1). The vector outline of the plaque, any pocket borders, the carved-edge profile, anything you carved on the CNC.
3. Keep the engrave details on a normal output layer (text, image, fill).
4. Place the carved plaque on the laser bed roughly where it'll go.
5. Frame using "Tool Layers Only" in the Live Framing options. The red dot now traces the T1 outline of where Lightburn THINKS the plaque is.
6. Adjust until the red dot traces the actual plaque edges: slide the plaque, OR move the design in Lightburn (arrow keys nudge in 1mm steps; Shift+arrow = 0.1mm).
7. Run the engrave. The detail lands exactly where the CNC features expect it.

Use a T2 layer for secondary registration features (e.g., a screw hole or center mark) that you want visible during framing but ALSO want to confirm separately from the main outline.

Method 2: Sacrificial outline jig (the no-software approach)

Faster on repeat jobs and dead-simple. You make a one-time custom jig by lasing the plaque's outline INTO a piece of sacrificial material (MDF, scrap plywood, or even a layer of painter's tape on the bed). The cutout becomes a registration pocket the plaque drops into.

1. Place a sheet of sacrificial material flat on the bed (3mm MDF works great; 6mm if you want a deeper pocket).
2. Lase only the plaque outline from your Lightburn file as a Cut layer. This creates a pocket / registration hole that exactly matches the plaque's silhouette. Cut all the way through OR engrave a deep groove if you don't want to perforate the sheet.
3. Drop the carved plaque into the cutout. It can only sit in one position, the silhouette pins it.
4. Now run the rest of your Lightburn file (the engrave details only, set the outline layer Output OFF since the plaque is already in position).
5. The engraving lands exactly where designed because the plaque is registered to the bed by its own outline.

For repeat work, save the sacrificial jig and reuse it. Tape it down so it doesn't shift between runs.

Workflow: full CNC → laser handoff

1. Design once, register everywhere. Build the entire plaque (CNC profile + engraved details) in a single CAD/vector file. Export the CNC paths to your CAM software AND keep the same file open in Lightburn. The geometric relationship between profile and detail must be locked at the design stage, fix it later and you'll be chasing alignment forever.
2. CNC the plaque first. Run the 3D carve, sand, finish-prep if needed. If the wood is going to get oiled or stained AFTER engraving, do that step LAST so the engrave lines stay crisp.
3. Move to the laser. Load the same master file in Lightburn, CNC features set to T1 (or pre-cut sacrificial outline jig in place).
4. Focus on the highest engrave surface. 3D plaques have multiple Z heights, the laser focal point should be on the surface where most of the detail lives (usually the recessed center). For plaques with engraving across multiple heights, sublayers with separate Z offsets handle the variation.
5. Frame, run, inspect. Pull the part, check alignment to the CNC features, finish.

Common pitfalls

• Plaque shifts mid-engrave. 3D plaques don't lay flat, they rock on their carved profile. Use double-sided tape or weight the plaque OUTSIDE the engrave area to lock it down.
• Focus drift across uneven surfaces. If the engrave area is recessed by more than ~3mm from the original Z surface, refocus before running, or split into sublayers with different Z offsets.
• Designed in two separate files. If the CNC paths and the engrave details were drawn in different files / at different scales, you'll never get them to register. Always master in one file.
• Sacrificial jig pocket too tight. Add 0.2-0.3mm clearance to the jig outline so the plaque drops in cleanly. Snug-but-not-pinched.
• Engrave bleeds onto a CNC bevel. Out-of-focus regions still mark, keep the engrave at least 2mm inside any sloped surface, OR mask the bevel with painter's tape.

Source: Kinetic Carving, CNC plaque finished on the CO2 laser; T1 / T2 Tool Layers and sacrificial outline jig as alternative alignment paths.