What is the Flat Depth option in V-Carve toolpaths, when should I use it, and how does the clearance tool work?

Overview

The Flat Depth option in the V-Carve toolpath form limits the maximum depth the tool will cut, creating a flat-bottomed carve instead of a pure V-groove that goes deeper as the design gets wider. This is one of the most important but frequently misunderstood V-carving settings. It is the same in VCarve Pro and Aspire.

How V-Carving Depth Works Without Flat Depth

A V-bit cuts deeper the wider the area it has to carve. For narrow vectors (small letters, fine details), the V-bit only cuts a shallow groove. For wide vectors (large letters, bold fonts), the V-bit must go deeper to reach both sides, potentially too deep for your material. With no Flat Depth, the toolpath carves to full depth, with multiple Z level passes calculated automatically where the tool must cut deeper than the Pass Depth set in the Tool Database.

Depth is determined by: vector width / (2 x tan(half the bit angle))

• A 90° V-bit needs to go 0.5" deep for a 1" wide channel
• A 60° V-bit needs to go 0.866" deep for the same 1" channel (cuts deeper)
• A 120° V-bit only needs to go 0.289" for the same 1" channel (cuts shallower)

To control depth without Flat Depth:

• Use a wider-angle V-bit (120° cuts shallower than 90°, which cuts shallower than 60°)
• Make the design smaller (narrower vector widths = less depth required)
• Use Flat Depth

When to Use Flat Depth

Thin material: V-carving large letters in 1/4" material would cut through. Setting Flat Depth = 0.20" prevents the bit from going deeper than that limit.

Consistent appearance: Wide and narrow elements in the same design carve to different depths. Flat Depth unifies the appearance by capping the maximum depth.

Clock faces, thin panels, signs on thin stock: Any time material thickness limits how deep you can go.

Carved into a pre-machined pocket: When V-carving into the bottom of a pocket, set Start Depth to the pocket depth (for example, to carve into the bottom of a 0.5" pocket, Start Depth = 0.5"). Then set the Flat Depth, and check the preview to confirm the flat bottom sits at the depth you expect.

What Flat Depth Does Visually

With Flat Depth enabled:

• Narrow parts of the design: still cut as a true V-groove (the bit doesn't reach the flat depth limit here)
• Wide parts of the design: flat bottom at the specified depth, with V-angled walls on both sides

The result is visually similar to a V-carve but with flat-bottomed areas in the wider regions. Some people prefer this look; others prefer the pure V-carve look without flat bottoms.

The Clearance Tools (Important for Quality)

When Flat Depth is enabled, there will be wide flat-bottomed areas that need to be cleared. If no clearance tool is selected, the V-carving tool clears the flat areas itself as well as doing the V-carving. That is inefficient and leaves poor surface quality, because the V-bit is doing heavy material removal that a flat end mill handles much better.

Best practice: add clearance tools for any significant flat area

1. Check Use Clearance Tools
2. Click Select and choose an end mill, ball nose or engraving cutter (for example a 1/4" or 1/8" end mill)
3. The clearance tool runs first to remove the bulk of the flat area, leaving an allowance for the V-carving tool
4. The V-bit then follows to cut the precise V walls and corners

You can add more than one clearance tool. The first tool in the list removes as much material as it can, and later tools only machine areas the earlier tools could not fit. For example, a 1/4" end mill first, then a 1/16" end mill for tight areas, leaves the V-bit even less heavy lifting. The order of the tools in the list should match the order they run on the machine.

Clearance tool options:

• Strategy: Offset or Raster for the first clearance toolpath (with a Raster Angle for Raster)
• Cut direction: Climb or Conventional for each clearance tool
• Ramp Plunge Moves: applies ramping to the clearance tool's plunge moves
• Corner Sharpen: raises the selected engraving tool to fit its smaller tip into narrower regions. It is available for a tool positioned second or later in the list

For raised letters specifically, consider the Prism Carving toolpath, which creates raised-letter profiles with angled sides. It is the mirror image of V-carved letters.

V-Bit Angle and Depth Control

Choose a wider-angle bit when material is thin or you need shallow carves. Use Flat Depth as a secondary control to prevent any bit from exceeding the safe depth limit.

V-Carve Depth Too Deep: Quick Fixes

1. Set Flat Depth (the easiest fix)
2. Switch to a wider-angle V-bit (from 60° to 90° or 120°)
3. Use a ball nose bit: the documentation says ball nose tools can also be used to V-carve. Their rounded tip changes how depth builds up, so test the result on scrap
4. Scale the design smaller: narrower vector widths mean shallower cuts
5. Engrave instead: use an engraving bit with a small flat at the tip. The flat limits the maximum depth naturally