How do I surface (flatten) my spoilboard, and which toolpath do I use?

Surfacing (also called flattening) your spoilboard is a maintenance procedure that affects cut quality and Z-depth accuracy. VCarve Pro and Aspire do not have a dedicated Surfacing toolpath button, but you can create one with a standard Pocket toolpath.

Why You Need to Surface

• Spoilboards develop grooves from profile cuts over time
• Spoilboards can bow or warp, especially MDF in humid conditions
• A non-flat spoilboard causes inconsistent cut depths, especially for V-carving
• Resurfacing removes high spots and creates a fresh, flat reference plane

How to Set Up a Surfacing Toolpath

Setup:

1. Create a new job sized to the area you can surface (your machine bed, less a margin).
2. Set Z Zero Position to Material Surface, and zero the bit on the top of the spoilboard at its highest point. Cut Depth in the Pocket toolpath is measured down from the material surface, so do not set Z zero to the machine bed for this job: the tool would run above the spoilboard and cut air.

Create the toolpath:

1. Draw a rectangle slightly smaller than your full machine cut area (leave about 1 to 1.5" margin from machine limits).
2. Create a Pocket Toolpath on this rectangle:

• Tool: A fly cutter or surfacing bit is common. A large end mill (1 to 1.5" diameter) also works.
• Strategy: Raster, with direction along the longest axis
• Cut Depth: 0.02 to 0.04" (0.5 to 1 mm), just enough to skim the surface flat
• Pass Depth: Same as Cut Depth (single pass)
• Stepover: 40 to 50% of bit diameter is common shop advice (more coverage per pass)

3. Calculate the toolpath and preview to verify it covers the full area.
4. Save with your standard post-processor.

Notes

• Try both cut directions on your spoilboard material and keep the one that leaves the cleaner surface.
• After surfacing, re-zero your machine Z to the new surface before cutting any real work.
• Some users add a second pass (for example 0.05" total depth, run twice) to guarantee a flat plane.
• For MDF spoilboards, some users seal with lacquer or shellac after surfacing to reduce moisture absorption.
• Surfacing bits (large flat-bottom insert cutters) generally leave a cleaner surface than spiral end mills.

Frequency (shop advice, adjust to your machine)

• Production shop: surface weekly or whenever Z-depth inconsistencies appear
• Hobby or occasional use: surface every 2 to 3 months, or whenever:
• Profile cuts don't go cleanly through in spots
• V-carve depth is inconsistent across a piece
• After any accidental deep cuts into the spoilboard

Job Templates for Surfacing

Many users save a permanent surfacing job file (VCarve Pro saves jobs as .crv, Aspire as .crv3d; a .crv3d file is only compatible with Aspire) with the surfacing toolpath already set up. Open it, select your surfacing bit from the tool database, and run, with no setup needed each time.