CAM Toolpaths Explained Profile Pocket V-Carve and 3D

What a Toolpath Is

After drawing your design in CAD, CAM (computer-aided manufacturing) software converts it into G-code — the actual movement instructions the machine runs. The type of toolpath determines how the bit moves through the material to achieve the desired result.

Choosing the wrong toolpath for a job is one of the most common beginner CNC mistakes. Here is what each one does.

Profile (Contour)

A profile toolpath traces the outside or inside of a vector path with the bit. The bit follows the line at a set depth.

Outer profile: cuts the outside of a shape, producing a part that falls free from the sheet. The bit center travels one tool radius outside the line.

Inner profile (pocket outline): cuts the inside of a closed shape, like a slot or mortise, leaving the shape standing.

On-path: bit center follows the line exactly. Used for marking or engraving lines.

When to use profile: cutting parts out of sheet material, cutting pockets with defined walls, cutting slots.

Key settings:

• Tabs: small material bridges left in the profile cut to hold the part in place until you remove it manually. Essential for preventing small parts from shifting and ruining the last pass.
• Lead-in/Lead-out: curved entry and exit paths that prevent the bit from plunging straight into the cut edge, reducing marks.
• Climb vs Conventional: climb cut (bit moves in the direction of rotation) generally gives better finish on wood. Conventional is more stable for aggressive cuts.

Pocket

A pocket toolpath removes all material inside a closed shape to a specified depth. The bit rasters or spirals back and forth, clearing the entire area.

When to use pocket: recessed areas, sign backgrounds to be painted or engraved into, drawer slides, housings, text relief.

Key settings:

• Stepover: how much the passes overlap. 40-50% of bit diameter for roughing, 5-10% for finishing.
• Roughing + finishing pass: rough with a large bit and aggressive stepover, then finish with a smaller bit or lighter final pass for clean surface.
• Ramp: instead of plunging straight down to depth, ramp in at an angle. Reduces load on small bits.

V-Carve

V-carving uses a V-shaped bit. The depth of cut varies with the width of the design — narrow strokes cut shallow, wide strokes cut deep. The result is a naturally tapered engraved line.

When to use V-carve: sign lettering, decorative designs, inlay preparation, any artwork where you want that hand-carved look.

Requires V-carve CAM software: VCarve Pro, Carbide Create, Carveco, Fusion 360 (2D Chamfer toolpath), or gSender's built-in V-carve. Standard profile/pocket toolpaths cannot do V-carving.

Key settings:

• Bit angle: 30°, 60°, or 90°. 60° is the most common for sign work. Smaller angle = deeper narrower cuts.
• Flat depth (for V-carve with flat bottom): sets a maximum depth, causing the V to flatly bottom out on wide areas rather than cutting infinitely deep.
• Combine with pocket: a V-carve + pocket combination uses a V-bit for the edges and a flat end mill to clear the center of wide areas. This is how most professional carved signs are made.

3D Contour

3D toolpaths follow the surface of a 3D model, moving in X, Y, and Z simultaneously to carve complex curved shapes. Used for relief carvings, decorative panels, and mold making.

When to use 3D: relief portraits, decorative panels, organic shapes, molds.

Two main passes:

1. Roughing pass: large flat or ball-nose bit removes bulk material quickly with aggressive stepdown
2. Finishing pass: smaller ball-nose bit at fine stepover traces the 3D surface

Key settings:

• Ball-nose bit: essential for 3D finishing — the round tip maintains contact with curved surfaces
• Stepover for finishing: 3-8% of bit diameter. Smaller = smoother surface but much longer job. 5% stepover on a 1/4" ball-nose takes 4-6× longer than 10% stepover.
• Direction: parallel (one direction), cross-hatch (both directions), radial (outward from center). Cross-hatch and radial give the smoothest results.

Drill and Bore

Plunges the bit straight down for holes. Drill cycles are fast for through-holes. Boring uses circular interpolation for larger or precise holes.

Which Software Supports What