1. The input: CL data and events
CAM systems produce cutter location (CL) data: tool tip positions, tool axis vectors, feedrates and a stream of events such as "tool change", "start of operation", "coolant on" or "drilling cycle". This data is machine-independent; it describes what to cut, not how a particular machine should move.
TOOL T1 D10 FLAT
SPINDL 9000 CLW
RAPID X-12.0 Y5.0 Z50.0 I0 J0 K1
FEDRAT 1200
GOTO X-12.0 Y5.0 Z-2.0
CIRCLE CENTER X0 Y5 RADIUS 12 CCW ...
CYCLE DRILL DEPTH 20 RETRACT 3 ...2. Event handling
The post is event-driven. Each CAM event calls a handler in the post: start of program, start of section/operation, tool change, rapid move, linear move, circular move, cycle point, end of section, end of program. The handler decides what code to output.
3. Inverse kinematics (multi-axis)
For 4- and 5-axis work, CL data contains tool axis vectors. The post (or the CAM machine configuration) converts each vector into rotary axis angles for the specific machine, chooses between multiple possible solutions, and, unless TCP is used, calculates the linear axis positions that account for pivot offsets.
4. Formatting
| Rule | Example |
|---|---|
| Decimal places and trailing zeros | X12.5 vs X12.500 vs X12.5000 |
| Decimal point required | X10. (on FANUC, X10 without a decimal point is read as 0.010 mm unless calculator-type input is enabled) |
| Units and scaling | mm / inch, degrees, feed per minute or per revolution |
| Line numbers | N10, increment, maximum |
| Comments | ( ) for FANUC, ; for Siemens |
5. Modal logic
Most G-codes and axis words are modal: they stay active until changed. The post only outputs what has changed, keeping programs short and readable, while forcing output where the machine requires it (for example after a tool change).
6. Cycles and machine features
Drilling events become canned cycles (G81, G83, G84 or controller equivalents) if supported, or are expanded into linear moves if not. The post also inserts machine features: high-speed machining modes, TCP, tilted planes, probing macros and clamping codes.
7. The output
N10 T1 M06
N20 G00 G90 G54 X-12. Y5. S9000 M03
N30 G43 H01 Z50. M08
N40 G01 Z-2. F1200.
N50 G03 X0. Y17. I12. J0.
N60 G81 X20. Y20. Z-20. R3. F300.
N70 G80The toolpath defines the part. The post processor defines how safely and efficiently the machine makes it.
Need a post that gets this right?
See our CNC post processor development service and why machines need specific posts.