From Model to Machine

Fabrication starts long before CAM - it starts in how you model. A model built only to look right on screen often cannot be made; a model built to be fabricated carries the process in its geometry. Practically, that means clean, closed geometry (a 3D print needs a watertight mesh - no holes, no flipped normals, no self-intersections; a solid model needs real solids, not loose surfaces), and it means modelling to real material.

If you are cutting 18 mm plywood, every slot, tab and thickness in the model should reference that actual measured sheet - not a nominal 18 mm, because a sheet sold as 18 mm often measures 17.4. If you are milling, avoid geometry a tool physically cannot reach: sharp internal corners, deep narrow pockets, undercuts a straight tool cannot see. The habit to build now is to model as the machine will make it: right thickness, reachable features, and joints sized for the process. A model that ignores the machine just pushes every problem downstream to the point where material and time are already spent.

There is a second, quieter benefit to modelling this way: the model stays editable. Drive thickness, kerf and tab sizes from named parameters or dimensions rather than baking them into fixed geometry, and when the real sheet measures 17.4 instead of 18 you change one number and the whole part updates. A parametric or history-based model (in Fusion 360, SolidWorks, or a Grasshopper definition) is worth far more to a fabricator than a dead lump of surfaces, because fabrication is iterative - the first cut teaches you something, and you want to fold that lesson back into the file in seconds, not rebuild it. Modelling for the machine and modelling to stay editable are the same discipline seen from two sides.

The file format is the passport between programs, and the wrong one loses information. The rough rule: meshes for additive, precise geometry for subtractive.

For 3D printing, you export a mesh - STL (triangles, the long-time default) or the newer 3MF (which also carries units, colour and materials). A mesh approximates curves with flat facets, so export at a fine enough resolution that the facets do not show, but not so fine the file becomes unwieldy. For laser and 2D routing you export vectors - DXF or SVG - clean, closed polylines at 1:1 scale, because the machine cuts exactly the lines you give it; stray double lines or open curves cause double-cuts or skipped paths. For CNC milling and anything needing true curves, export STEP (or IGES) - a precise boundary representation that keeps arcs as arcs, not as chords. Two things trip everyone: units (a model exported in inches and read as millimetres comes out 25.4 times too small - always confirm), and scale/origin (export at 1:1 with a sensible origin). Check the exported file in a viewer before you trust it; a two-second look catches most disasters.

The deeper distinction underneath the file extensions is mesh versus solid. A mesh (STL, OBJ, 3MF) is a skin of flat triangles - light, universal, but an approximation with no true curves and no editable history, so once it is a mesh it is hard to change. A solid or boundary-representation model (STEP, native CAD) carries exact geometry the CAM can offset and analyse precisely. As a rule, stay in precise solid or vector geometry as far down the pipeline as you can and convert to mesh only at the last moment, for the process that needs it - that keeps your options open and your dimensions honest. And whatever you export, name and version the file clearly; a workshop full of finalfinalv3.dxf files is a workshop about to cut the wrong one.

CAM - computer-aided manufacturing - is where a shape becomes a plan. Programs like Fusion 360, RhinoCAM, VCarve or Mastercam take your exported geometry and let you answer the questions the model cannot: which tool (a 6 mm flat end mill, a 60-degree V-bit, a 0.4 mm print nozzle), how fast to feed and spin (feed rate and spindle speed), how the tool should travel (the toolpaths of the next lesson), and in what order. You define the stock - the block or sheet you are cutting from - so CAM knows what is solid and what is air, and you build or pick from a tool library so its calculations match the real cutter in the machine.

CAM then generates toolpaths and, crucially, simulates them - a coloured animation of the tool removing material - so you can catch a plunge into a clamp or a gouge before it happens in aluminium. Finally a post-processor translates the generic toolpath into the specific dialect of G-code your machine reads, because a Haas mill, a GRBL router and a Prusa printer all speak slightly different flavours. CAM is the difference between a shape and a runnable job.

Here is the single idea that ties everything together: the machine and your model must agree on where zero is. A machine thinks in X, Y and Z - a right-handed coordinate system. It has its own fixed machine coordinates (often called G53), set by its home switches. But your part is not bolted to the machine home; it sits wherever you clamped it. So you define a work coordinate system - a work origin, commonly G54 - by touching the tool to a chosen point on the actual stock and telling the machine this point equals model zero.

Everything the toolpath does is measured from that origin. Set it on a corner of the sheet, a dowel-pin datum, or a machined feature - but choose something repeatable, so that if you flip the part or run a second sheet, the origin lands in the same place. Get the work origin wrong and the whole job shifts: the part is cut in the right shape but the wrong place, off the edge of the stock, or into a clamp.

Setting the origin has real technique behind it. In X and Y you touch off an edge, use an edge-finder or a probe, or register the stock against fixed dowels; in Z you decide whether zero sits on the top of the stock (common, so cut depths read as negative numbers into the material) or the bed (so a cut-through path is safe even if the stock is thinner than expected). On a mill you must also account for tool length offsets, because each tool in the changer is a different length - the machine measures or you set how far each sticks out, so a tool change does not plunge the new tool too deep. And this is why fixturing matters as much as the origin - the stock must not shift mid-cut, or the material drifts out from under a correct toolpath. Model zero, work origin, tool offsets and a solid fixture together make one promise: that the geometry lands on the real material exactly where you designed it.

The last artefact of the handover is the setup sheet - the one-page summary CAM produces (or you write) that lets someone, including future-you, run the job without guessing. It lists the stock size and material, where the work origin is, every tool in order with its number and the feeds and speeds, the total run time, and any notes (flip halfway, change to the V-bit at operation three, watch the clamp on the left).

A good setup sheet is what separates a one-off you got lucky with from a process you can repeat and hand to someone else. It is also your safety net: reading it aloud against the machine before you press start - right tool loaded, origin set, stock clamped, nobody in the path - catches the mistakes that turn expensive. Fabrication is a team relay, and the setup sheet is the baton.