How does the Chamfer Toolpath work in VCarve Pro & Aspire for cutting beveled edges and countersinks?

Overview

The Chamfer Toolpath cuts a beveled edge along selected vectors using a V-bit or ball nose tool. It's ideal for decorative chamfered sign edges, countersunk holes, angled frame borders, and any design requiring a clean angled transition between two surfaces. It is available in both VCarve Pro and Aspire.

Tool Options

V-Bit

When a V-bit is selected, the chamfer angle is automatically fixed at half the included tool angle. A 90° V-bit produces a 45° chamfer. The angle cannot be manually overridden when using a V-bit.

Overcut Distance: Offsets the tool tip away from the work surface, using the side edge of the V-bit rather than the tip. This prevents the tip from leaving a witness mark (a fine scratched line at the bottom of the chamfer). Always verify the tool's cutting edge length is long enough to accommodate the overcut distance.

Ball Nose / Round Tool

When a ball nose or round tool is selected, the chamfer angle must be specified manually. The software approximates the angled chamfer using a series of fine passes that follow the slope. The smaller the tool's pass depth, the smoother the chamfer curve.

Key Settings

Chamfer Type (Inside/Outside & Direction):

• Outside Chamfer Down: Chamfer is outside the vector, sloping downward away from the vector. This is the classic sign-edge bevel
• Outside Chamfer Up: Chamfer is outside the vector, sloping upward toward the vector
• Inside Chamfer Down: Chamfer is inside the vector, sloping downward into the shape
• Inside Chamfer Up: Chamfer is inside the vector, sloping upward out of the shape
• Both Inside and Outside can be combined in one toolpath to create different chamfer profiles

Width: Horizontal size of the chamfer (how far the bevel extends from the vector edge)

Cut Depth: Vertical height of the chamfer. When Angle is set, adjusting Width automatically adjusts Cut Depth proportionally, and vice versa.

Max Cut Depth (read-only): Shows the full depth the tool will reach, including any overcut. Use this to verify the tool won't cut deeper than the material.

Start Depth: Where the top of the chamfer begins. Use 0 for surface-level chamfers. Enter the pocket depth if chamfering the edge of a recessed area.

Workflow

1. Draw or select the vectors defining the edge or shape to chamfer
2. Open Chamfer Toolpath from the Toolpaths tab
3. Select the V-bit or ball nose tool
4. Choose the Chamfer Type (Inside/Outside and slope direction)
5. Set Width and Cut Depth (or let one drive the other via the angle relationship)
6. Set Start Depth if needed
7. Set Overcut Distance if using a V-bit (recommended to avoid tip witness marks)
8. Calculate

The 2D Preview

The Chamfer toolpath generates a 2D preview in the canvas showing directional arrows on the vectors. The arrows point in the direction of the downward slope. Use this to verify the chamfer is on the correct side before cutting.

Common Use Cases

• Sign edge chamfer: Select the sign's outer profile vector and apply an Outside Chamfer Down to create a clean beveled edge all around the sign
• Countersunk hole: Draw a circle at the screw head diameter and apply Inside Chamfer Down to create a countersink recess
• Decorative frame border: Chamfer the inside edge of a routed frame for an architectural moulding effect
• Layered sign bevel: Chamfer the boundary between two layers of a multi-layer sign for a shadow-line effect