Why did my V-carve cut deeper than the preview showed, and why is one end of the sign deeper than the other?

Why this happens

V-carve depth is extremely sensitive to the distance between the bit and the material surface. If the actual surface isn't exactly where the software thinks it is, depth error shows up immediately. Because a V-bit gets wider as it goes deeper, even 0.02" of surface error visibly fattens every letter.

The four usual causes, in rough order of likelihood:

1. Material isn't flat or uniform thickness. A cupped or thickness-varying board carves deep where the surface is low and shallow where it's high (the classic "deeper at one end" symptom).
2. Z-zero was set inaccurately or on the wrong reference (see the Z-zero setup entries).
3. The V-bit's real angle doesn't match the tool database. A mislabeled or worn bit changes the geometry.
4. Machine/spindle not trammed (not perpendicular to the bed).

The fix

1. Surface the board first. Run a skim or surfacing pass over the carve area before V-carving (shop advice: a very light pass, roughly 0.001 to 0.01" deep). This is often the biggest improvement for V-carve consistency, because it makes the surface match Z-zero everywhere.
2. Check what the software intended: run Preview Toolpaths and inspect the widest areas of the design. If the simulated depth looks correct, the G-code is correct, and the problem is machine-side (Z-zero, flatness, tram, lost steps). Stop editing the toolpath and check the machine.
3. Verify the bit angle: cut a shallow test groove, measure depth against width, and compute the real included angle. If it differs from the tool database entry, create a custom tool with the true angle.

Pro tips

• Zero Z in the middle of the carve area, not at a corner, to average out small flatness errors.
• For thin material where you can't afford a surfacing pass, zero on the machine bed instead and let the measured thickness drive the math.