Machine coordinates, work coordinates, home and zero
Home is a fixed physical place the machine finds by itself, and it never moves. Zero is where YOU tell the machine your material starts, and it changes with every job. G-code is written in work coordinates, measured from your zero. Set zero wrong and everything cuts in the wrong place, perfectly.
Two different systems, and why both exist
Machine coordinates describe the physical machine. Machine zero, usually called home, is a fixed corner of the machine's travel that it finds by itself using limit switches. It is the same place today and next month. The machine uses it to know where its own limits are.
Work coordinates describe your material. Work zero is a point on your workpiece that you choose and tell the machine about. Every toolpath is written relative to that point. If your design has a hole at X 2, Y 3, the machine puts it two inches right and three inches back from your zero, wherever you put it.
The separation is what makes CNC practical. Your G-code does not care where on the table you clamped the wood. You just tell the machine where the wood starts, and the same file works anywhere on the bed.
Setting XY zero
Whatever corner your CAM software used as the design origin is where you set XY zero on the material. The common choices:
| Origin | Good for | Watch out for |
|---|---|---|
| Front left corner of the stock | Sheet goods, anything where you cut from a known corner | The corner must be square and you must find it accurately |
| Centre of the stock | Round things, medallions, a design centred on a slab | Finding the true centre of an irregular blank takes a moment |
| A specific feature, like an existing hole | Second operations and repairs | You are trusting the accuracy of the first operation |
Set XY zero the same way your design was set up. This sounds obvious and it is the single most frequent cause of a cut landing off the edge of the material.
Setting Z zero, and the choice that trips everyone
Z zero can be either the top of the material or the spoilboard surface, and the toolpath was written expecting one of them.
| Top of material | Spoilboard | |
|---|---|---|
| Best for | Most work: carving, pockets, V-carving, 3D | Cutting all the way through sheet goods |
| Advantage | Carve depths are exactly what you asked for, regardless of stock thickness | Cut-through depth is exact even if the board is thicker in places |
| Risk | Stock thicker than the file thinks means the profile does not cut through | Every carve depth depends on the stock thickness being exactly right |
Touch plates and probes
A touch plate is a conductive block of a known thickness. The machine lowers the bit until it makes electrical contact, then sets zero accounting for the plate thickness. It is faster and far more repeatable than the paper method, and it is the single best early upgrade for most machines.
Two things people get wrong with them:
- The magnet clip has to be on the bit or the collet, not just anywhere on the machine. The circuit is bit to plate. If your machine has a painted or anodised gantry, clipping there may not conduct.
- The plate thickness in the configuration has to match the plate. If your probe results are consistently off by the same amount, that number is usually why.
Without a probe, the paper method works: lower the bit in small steps with a piece of paper under it, until the paper just drags. That puts you about one paper thickness high, which is close to 0.004 inches, roughly 0.1 mm. Either account for it or accept it, but know it is there.
Keeping it straight in your head
Say it out loud before you press start:
- "XY zero is the front left corner of the board, and the file was drawn from the front left corner."
- "Z zero is the top of the board, and the file expects the top of the board."
- "The tool in the collet is the tool the first toolpath asks for."
Three sentences. They prevent most of the ruined workpieces in hobby CNC.
When zero gets lost mid-job
If the machine loses position during a cut, the work coordinate system is still valid but the machine no longer knows where it is within it. On a machine with homing switches you can re-home and the work zero is usually recoverable, because the controller stores it relative to machine home. On a machine without homing, it is generally gone. That difference is most of the argument for having limit switches.