CAM & Toolpaths

Most subtractive jobs are built from a small set of toolpath types, and naming them is half the battle. A profile (or contour) path follows an outline - the outside edge of a part, or the inside of a window - with the tool offset to one side by its radius so the finished edge lands on your line. A pocket (or area-clearance) path removes all the material inside a boundary down to a depth, sweeping back and forth or spiralling inward; this is how you carve a recess, a tray, an inlay. A drill cycle plunges holes at marked points, often with peck cycles that retract to clear chips.

For anything with real 3D form, the job splits into roughing and finishing. Roughing hogs out the bulk quickly with big stepdowns and a tolerance for a rough surface - it just needs to get most of the waste gone, leaving a small even layer of stock behind. Finishing then takes light passes that trace the final surface closely for a clean result. You almost always rough first (fast, ugly) and finish last (slow, precise), and often add an intermediate semi-finish pass for tall or detailed parts so the finishing tool meets an even amount of material everywhere. Read a CAM tree and you are reading this vocabulary: profile, pocket, drill, rough, semi-finish, finish, in a deliberate order.

That order is not cosmetic - it is planning. You rough with a big, stiff tool for speed, then switch to a smaller tool for detail the big one could not reach. You cut holes that other features register to before you free the part from the stock, while it is still held rigidly. You leave the thin, delicate features until last so they are supported as long as possible. A well-built CAM tree reads like a recipe written in the right sequence, and a big part of becoming fluent is learning to order operations, not just create them.

Two settings do more than any others to trade speed against quality. Stepover is how far the tool shifts sideways between adjacent passes - how much of its diameter bites each time across. A big stepover (say 80-90% of tool diameter for roughing) clears material fast but leaves ridges; a small stepover on a finishing pass (10-20%, or less for a ball-nose on a curved surface) leaves a smooth surface but multiplies the number of passes and the time.

Stepdown (or depth of cut) is how deep the tool goes per layer. Take too much at once and you overload the tool - it deflects, chatters, or snaps; take a little at a time and you are safe but slow. A rough guide many people start from for milling is a stepdown of half to one tool diameter and adjust by material and machine rigidity. On a curved 3D finish, the leftover ridges between passes are called scallops, and scallop height falls as stepover shrinks - which is exactly why a mirror finish costs time. Worked example: a 6 mm ball-nose at 0.3 mm stepover leaves far smaller scallops than at 2 mm, but needs roughly seven times as many passes to cover the same width. Choosing these numbers is the craft.

Modern CAM softens the old trade-off with smarter clearing strategies worth knowing by name. Adaptive (or trochoidal) clearing keeps the tool engaged at a constant, controlled load by cutting in curved, looping arcs rather than straight full-width passes; that lets you take a deep stepdown but a light radial bite, so you hog material fast without overloading or overheating the tool - often faster and kinder to the tool than a conventional heavy pass. How the tool enters the cut matters just as much: plunging a flat end mill straight down like a drill is hard on it, so CAM ramps in on a shallow slope or spirals down into a pocket, spreading the load. These entry moves - ramps, helical plunges, lead-ins - are not decoration; they are why one program runs clean and another chatters or snaps a cutter on the first plunge.

Direction matters. In climb milling, the cutting edge moves in the same direction as the tool is fed, so each tooth starts in thick material and thins to zero - on a rigid machine this gives a cleaner edge, less rubbing and longer tool life, and it is the usual default on CNC. In conventional milling, the edge moves against the feed, starting thin and thickening; it can be safer on flimsy or backlash-prone setups but tends to leave a rougher finish. Knowing which you have chosen explains a surprising number of edge-quality mysteries.

Underlying all of it are feeds and speeds - the feed rate (how fast the tool travels through material) and spindle speed (how fast it spins). These come from the material, the tool and the machine, and the goal is the right chip load: each tooth should peel a proper chip, not rub (which overheats and dulls the tool) nor bite off more than it can clear. Tool makers publish starting numbers; you tune by sound and chip. Too slow a feed with too fast a spindle is the classic beginner error - it burns wood, melts acrylic and work-hardens aluminium. The tool should cut, not polish.

Before a single line of code reaches the machine, run the CAM simulation. Every serious CAM package animates the toolpath removing material from your stock, in colour, at any speed, and it is the cheapest insurance in fabrication. You are watching for a short list of expensive mistakes: the tool plunging into a clamp or the bed, a rapid move dragging through stock it should have flown over, a pocket cutting deeper than the material is thick, gouges where the tool is too big for a detail, and collisions between the tool holder and tall features.

Simulation also gives you the honest run time and lets you sanity-check the order of operations - are you finishing a face before drilling the holes that reference it? It is also where you plan how parts stay put as they are freed: when a profile cuts all the way through, the part can come loose and get flung or re-cut, so CAM leaves small tabs (little uncut bridges to the surrounding stock) or you use a vacuum bed or tape to hold it, and you trim the tabs by hand afterwards. Watch, too, for lead-in and lead-out moves that ease the tool onto and off the cut line so it does not leave a witness mark where it plunged straight in.

On a laser or router, a dry run - the head tracing the path in the air, or at zero power - is the physical equivalent of the on-screen simulation. The rule is simple and non-negotiable: nobody who values their tools, their material or their fingers sends an unsimulated job. And simulation is never a substitute for real safety - guards, extraction, eye protection, training and supervision on powered machines still apply, every time.

When the toolpaths are set and simulated, CAM posts them: the post-processor converts the generic path into the exact G-code dialect your machine speaks and writes the file you will load. This is the moment the abstract plan becomes concrete instructions - G0 rapids to position, G1 feed-cuts to coordinates, M3 starts the spindle, M6 calls a tool change, G54 selects your work origin.

The key discipline is matching the post to the machine: a file posted for a Haas mill will not run correctly on a GRBL router, and a printer wants sliced G-code from a slicer, not mill code. Load the posted file, confirm the machine reads it, verify the work origin one last time, and only then run. A toolpath is a plan; posted G-code is the plan in the machine's own words - and the last thing you check before metal meets material.