How does the V-Carve Toolpath work in VCarve Pro & Aspire: flat depth, clearance tools, and start depth?

Overview

The V-Carve Toolpath uses a V-bit to carve designs where the depth of cut varies automatically based on the width of the vector at each point. Wide areas receive deeper cuts; narrow areas receive shallower cuts. The result is crisp, sharp-cornered engraved text and art that looks hand-carved. This is the defining toolpath for decorative CNC signmaking. It is the same in VCarve Pro and Aspire.

How V-Carving Works

The software calculates the exact depth at every point along the vectors from the tool angle and the width and shape of the vectors, so the V-bit just touches both walls of the design. In narrow strokes (like the top of a serif letter), the bit barely grazes the surface. In wide open areas (like the center of a large letter O), the bit goes to its greatest depth. The result is a continuously varying depth cut that produces the characteristic V-carved look.

Key Settings

Start Depth (D)

The depth at which V-carving begins. Usually 0 for carving from the surface. Use a non-zero Start Depth to V-carve into the bottom of an existing pocket. Example: if the pocket is 0.5" deep, set Start Depth = 0.5" to carve into the pocket floor.

Flat Depth

By default, V-carving goes to whatever depth produces crisp corner-to-corner contact. For wide open designs this can be very deep. Flat Depth limits the maximum depth the tool will machine to. Any region too wide for the V-bit to fill within the flat depth limit is carved flat at that depth instead.

Use cases for Flat Depth:

• Creating flat-bottomed V-carved letters (more of a wood router sign style than pure V-carving)
• Controlling maximum depth when material is shallow
• Artistic preference for a mix of V-carved edges with flat centers

Clearance Tools (Flat Area Clearance)

When Flat Depth is set, clearance tools can be added to efficiently remove material from the flat areas before the V-bit does the detail work. This matters for efficiency on large flat designs: without it, the V-bit would have to clear the flat areas itself (very slow).

How to set up:

1. Check Use Clearance Tools
2. Add one or more end mill, ball nose or engraving tools from the Tool Database
3. 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. Every clearance tool leaves an allowance for the V-carving tool
4. The V-bit does the final sharp detail pass

Strategy (Offset or Raster): Controls how the first clearance tool fills the flat areas. Same options as the Pocket Toolpath.

Ramp Plunge Moves: Optionally ramps the clearance tool's plunges to reduce impact on the tool and material.

Corner Sharpen: For a second or later tool in the list, raises a smaller engraving tool to fit its tip into tight corners the larger tool could not reach, which gives sharper corners in flat areas.

Workflow for a V-Carved Sign

1. Draw or import all vectors (text, borders, decorative elements)
2. Select all vectors to V-carve
3. Open V-Carve Toolpath
4. Select a V-bit (commonly 60° or 90°)
5. Set Start Depth = 0
6. For flat centers: enable Flat Depth, set the depth, and add a clearance end mill
7. Calculate
8. Simulate and verify the carved result looks correct
9. Add a Profile cutout toolpath for the sign outline

V-Bit Selection Impact

Narrower angles produce more dramatic V-carving with deeper cuts in wide areas. Wider angles produce more subtle, shallower results.

V-Carve vs V-Carve + Flat Depth: Side by Side

Project Toolpath onto 3D Model

When a 3D model has been defined in the job, you can check Project toolpath onto 3D Model. After the toolpath is calculated, it is projected down in Z onto the surface of the model. The carving follows the model's contours, which suits carving text onto a curved plaque or decorative elements on a shaped sign blank. The projected depth is limited so it does not exceed the bottom of the material.