What the checker interprets
The interpreter follows RS-274/NGC conventions used by Grbl, LinuxCNC, Fanuc-style and Mach controls: G20/G21, G90/G91, G90.1/G91.1 arc centers, G17–G19 planes, G0–G3 including helical and R-format arcs, G54–G59.3, G10 L2, G92, G53, G28/G30 with intermediate points, G43/G43.1/G49 tool lengths, tool changes, spindle state and G73/G81–G89 canned cycles with G98/G99 retract. Arcs are checked with their real swept extents, not just endpoints.
Work coordinates versus machine coordinates
Soft limits live in machine coordinates. Your program lives in work coordinates. Machine position = programmed position + active work offset + any G92 shift (+ tool length on Z with G43). Enter the offsets your controller shows for each work coordinate system; a missing or stale offset is the most common reason a proven program suddenly alarms.
Keep-outs, safe Z and stock
Keep-out boxes model vises, clamps, fixtures or a rotary table. Give them in machine coordinates (fixed to the table) or in a work frame (moving with the part). Every straight move and arc chord is tested for entry. Separate checks flag XY rapids below your safe Z, rapid moves that end below the stock top, and feed moves below the stock while the spindle is off.
Safety boundary
This is a pre-run analysis aid, not a machine simulator or collision-avoidance system. It does not model the tool, holder or spindle body, machine kinematics, acceleration, rotary axes, cutter compensation (G41/G42), macro variables, subprograms, controller-specific canned-cycle variants or homing direction. Starting position is assumed at machine zero until the program sets all axes. Always dry-run above the part with reduced feed and rapid override, and keep a hand on feed hold.
Frequently asked questions
Why does my CNC raise a soft-limit alarm when the G-code looks fine?
Soft limits apply in machine coordinates. The active work offset, any G92 shift and the tool length decide where the machine actually travels. Enter those values to see which line leaves the envelope.
How do I get my machine envelope?
Use your controller’s soft-limit settings. For Grbl, paste the $$ output; $130–$132 become the default negative machine space.
Why is an XY rapid at my retract plane flagged?
Rapids between holes at a low R plane are normal for G99, but they are flagged when that plane is below your safe Z. Lower the safe Z to your R plane if that is intentional.
Is my G-code uploaded?
No. The program is interpreted in a Web Worker inside your browser.
Authoritative references
The LinuxCNC G-code reference and coordinate-system documentation describe modal groups, offsets and canned cycles. Grbl documents $130–$132 maximum travel and soft limits.
Browse machining tools · Audit Grbl settings · Calculate G-code arcs