CAM Toolpaths Explained: Profile, Pocket, V-Carve, and 3D

What Is CAM? CAM (Computer-Aided Manufacturing) is the step between your design and your machine. You feed a design into CAM software, define how you want to cut it, and CAM generates the G-code that the machine runs. Understanding toolpaths is understanding your options. -- Profile (Contour / Outside Cut / Inside Cut) The profile toolpath traces the outline of a shape with the router bit. Outside profile: cuts around the outside of a shape, leaving the shape. Used to cut a part free from sheet material. Inside profile: cuts the inside of a hole or cavity. Used to create a pocket with walls. On-line: centers the bit exactly on the path. Used for edge work. Critical consideration: The bit has a diameter. An outside profile needs to offset the path outward by half the bit diameter so the cut happens at the right place. Most CAM software does this automatically when you specify inside/outside. Tabs: Small uncut sections that keep the part attached to the sheet during cutting. Without tabs, the cut-free part can shift and ruin the final cut. In VCarve and Fusion 360, add tabs when cutting parts free from sheets. -- Pocket A pocket removes all material inside a defined area down to a specified depth. The bit follows the outer profile then sweeps back and forth (raster) or in offset rings (offset clearing) to remove the interior. Raster pocketing: back-and-forth rows. Efficient for large areas. Offset pocketing: concentric inward rings. Better for rounded shapes, less witness lines. Depth: set in multiple passes (DOC per pass) to avoid overloading the bit. When to use pocket: any operation where you remove material from a surface — inlay recesses, decorative carving, signage, living hinges (partial-depth pockets). -- V-Carve V-carve uses a V-shaped bit and cuts at varying depths based on the width of the design. Narrow areas: shallow cut. Wide areas: deeper cut. The result is a carved groove that precisely follows the original design outlines. V-carve is ideal for: lettering, decorative borders, wood burning look, traditional sign carving style. Common angles: 30°: Very narrow, fine detail, small text 60°: Standard — most sign lettering 90°: Wide, bold lettering, chamfers Flat pocketing combined with V-carve: for large letters, V-carve does the detailed edges while a flat bit clears the background. This is called "V-carve with flat clearing" in VCarve Pro. V-carve requires: a dedicated V-carve toolpath in your CAM software (VCarve, Carbide Create, Carveco, Fusion 360's Engrave toolpath). You cannot simulate V-carve with a regular profile toolpath. -- 3D Contour / Surface Machining 3D toolpaths follow a curved surface, cutting at varying Z heights to create smooth organic shapes. Roughing: a flat or bull-nose bit removes most material fast using horizontal slices. Large DOC, large stepover (40-60%). Finishing (scallop): a ball-nose bit follows the surface in fine passes. Small stepover (3-8%) for smooth finish, more time. Finishing (parallel): passes parallel to one axis. Faster than scallop but direction-dependent — better along the grain. Finishing (contour): follows Z-height contours like a topographic map. Good for terrain-like shapes. Software for 3D: Fusion 360 (free for hobbyists), VCarve Pro + Aspire, Carveco, MeshCAM. Basic CAM tools (Carbide Create free) don't support 3D toolpaths. -- Toolpath Order: Why It Matters Correct order: 1. Interior pockets first — before cutting the outside profile, machine any holes or recesses while the part is still attached to the sheet 2. Profile cuts last — cutting the outline last means the part is held firmly during all previous operations 3. Roughing before finishing — rough out material fast, then clean up with a slow precision finishing pass Wrong order creates problems: if you cut the outline first, the freed part shifts during subsequent operations. -- Conventional vs Climb Cutting Conventional (up-cut): bit rotation pushes chips toward the cut direction. Traditional, works in all machines. More tool pressure. Climb (down-cut): bit rotation pushes chips away from the cut direction. Produces better surface finish, less force on the workpiece. Can cause bit deflection if machine is not rigid — not recommended for very light hobby machines. In practice: rough in conventional, finish in climb for the best surface quality on hobby CNC.

Related Guides

Loading_