Post-processors

A post-processor turns Chipload’s toolpath into the G-code dialect your controller reads. Three are built in:

The LinuxCNC and Mach3/4 posts haven’t been run on a real controller yet. Their programs say so in a header comment: check the program and air-cut before you cut. If you run one of them successfully, please report it.

Every post writes arcs as G2/G3, mm and absolute coordinates, and waits 3 s after starting the spindle. The post-processor reference lists every post’s settings.

Choosing the post

• App: Job settings > Machine > Post. The list shows the built-in posts, then yours.
• Command line: chipload post use part.chipload --post linuxcnc.
• Machine profile: a profile names its post, and a project made from the profile gets it.

Your own post

A post is two files in the posts folder of your settings folder:

• NAME.toml, the settings (reference);
• the template the settings name (template = "NAME.nc.j2"), a Jinja text that writes the program.

The easiest start is a copy of a built-in post, from the crates/chipload-post/posts/ and templates/ folders of the source. Rules:

• Names: a post can’t take a built-in name (grbl, linuxcnc, mach3).
• Copied into the project: a project that uses your post keeps its own copy of both files, so it gives the same G-code on another computer or after you change the files. When your files differ from the project’s copy, the app shows Update next to the Post box (command line: run post use again).
• Sandboxed: the template sees only the values below, can’t read files, and stops with an error if it loops without end.
• The checker still decides. Whatever your template writes, the checker reads it back as a controller would. It accepts only the codes it knows: G0–G3, G4, G17, G20, G21, G90, G91.1, G94, the setup codes G40, G49, G80, G54, G61 and G64 P (at most 0.05 mm), M3–M6, M7–M9 and M30, and % lines. Anything else, such as G41/G42 cutter compensation, G43 tool lengths, G28 or G53 machine moves, or G91 relative moves, makes the check fail, and nothing is exported.

chipload post list shows every post and why one can’t be used, and chipload post show NAME what one writes (extension, decimals, arcs, tool changes). In the app they are under This computer > Post-processors in the Browser. chipload render writes a bare toolpath through a post, for trying a template (the result isn’t checked: use run to cut).

What the template sees

Numbers come already formatted in the program’s units: with the settings’ decimals in mm, inch_decimals (4 if missing) in inches.

Inches. A post writes inch G-code only if its settings say its template can: units = ["mm", "inch"], and the template writes {{ units_word }} where it would write G21. A post without units writes mm only, and a project whose machine is set to inch is refused with that post, so a template that writes G21 itself never gets inch numbers.

The built-in GRBL template shows how they fit together:

{{ units_word }} G90 G17 G94
{{ "M3" if spindle == "cw" else "M4" }} S{{ rpm }}
{% if dwell is not none %}G4 P{{ dwell }}{% endif %}
{% for s in segments %}
{% for m in s.moves %}
{% if m.comment is not none %}
({{ m.comment }})
{% endif %}
{{ m.code }}{% if m.x is not none %} X{{ m.x }}{% endif %}{% if m.y is not none %} Y{{ m.y }}{% endif %}{% if m.z is not none %} Z{{ m.z }}{% endif %}{% if m.i is not none %} I{{ m.i }} J{{ m.j }}{% endif %}{% if m.f is not none %} F{{ m.f }}{% endif %}
{% endfor %}
{% endfor %}
M5
M30