CAM post processor for Fusion 360 and the V1 Engineering MPCNC / LowRider family of machines. This is a modified fork of guffy1234/mpcnc_posts_processor, originally forked from martindb/mpcnc_posts_processor.
This is the v4.0 (Beta 3) post processor, distributed as the single file
MPCNC_v4.0_Beta3.cps.
Supported firmware (set by the Job → CNC Firmware property):
- Grbl — GRBL 1.1, and FluidNC, which this post treats as GRBL throughout
- Marlin — Marlin 2.x. Read from source at 2.0.9.7 and 2.1.2.5; nothing below that was read, so 2.0.9.7 is the floor every Marlin claim here rests on
- RepRap — RepRapFirmware (Duet3D)
- Repetier 1.0.3 is untested; its g-code is Marlin's, so choose Marlin
| Read this | |
|---|---|
| One part, one tool, zeroed by hand. You jog to your corner, post, and cut. | Hobbyist guide — seven settings matter; the rest can stay as they ship |
| Several operations, more than one tool, or several parts on their own fixtures. | Pro guide — work offsets, the machine travel height, tool-change hand-over, the validation guards |
| Looking up one setting. | Property reference — all 62, in dialog order |
At its core the post turns a Fusion CAM program into g-code for a hobby-class CNC (MPCNC, LowRider, and similar GRBL/Marlin/RepRap machines). Beyond the usual translation it is built around one central idea that shapes every other feature:
These machines are work-relative. Most of them have no reliable machine-Z reference — no tool setter, no tool-length offset register, often no Z endstop, sometimes no endstops at all. So the post does not lean on the machine frame. Instead you establish a work zero (by jogging to it, or by probing a touch plate), and everything the post emits — cutting, retracts, traverses between parts — is measured relative to that zero. Where a machine can home, homing buys repeatability and one job-level travel height, never the everyday Z cutting reference.
Two consequences run through the whole post, and knowing them explains most of the dialog:
- The post commands a work offset and can never read one back. It always knows which register is active, because it selects it itself at job start over whatever your sender left modal. It never knows where that register points — register contents are runtime state in the controller and there is no round trip. So every mode that uses a stored origin trusts it, and the shipped defaults establish an origin rather than trust one.
- The post changes no tool, on any firmware. A measured tool change needs a probe, a subtraction and a register to hold the result, and the post has none of the three. Its whole role at a change is to arrive correctly, hand over, and resume correctly.
The post is designed to degrade gracefully:
- A one-part, one-tool job needs almost no setup. Jog to your zero, accept the defaults, post, run.
- A larger job — many operations, more than one tool, or several parts on separate fixtures — has the extra structure available and validated, without complicating the simple case.
Other capabilities: 3-axis milling and jet (laser / plasma / waterjet) operations; canned drilling cycles expanded into plain moves; arcs; 3 laser power levels; two configurable coolant channels; four comment levels with a full property dump at the head of every file; optional line numbers; external include files for custom g-code. Only 3-axis toolpaths are supported — multi-axis operations are rejected with a clear error.
Units: the post outputs in whatever units the Setup uses (mm or inch), but every dimension in the dialog is entered in millimetres. The head of each posted file echoes the values the post resolved — in output units — so you can check them before the machine moves.
The post is a single file, MPCNC_v4.0_Beta3.cps.
- In Fusion, choose Manage → Post Library.
- Select My posts/Local in the sidebar.
- If an older copy is installed, select it and use the trash-can icon to remove it first. Beta 3 has a different filename from Beta 2, so an old copy will sit alongside it rather than being replaced, and the two are hard to tell apart in the picker.
- Use the Import icon to import
MPCNC_v4.0_Beta3.cps(or the latest version available). - Close the dialog.
- When posting, select Choose from library... and select this post.
- Review and set the properties as needed — start with the guide for your kind of job, above.
Beta 2 gave each part its own zero. Beta 3 corrected where those zeros come from, rebuilt tool changes around what the post can actually do, and — for the first time — ran the post against Autodesk's own engine instead of reasoning about it.
Two things to do before your first Beta 3 job, neither of them optional:
- Your saved settings will not carry over. Every property key in the dialog was renamed, so a Beta 2 preset falls back to its shipped default on every setting. Walk the dialog once, and look hardest at groups 4, 5 and 6 — those changed most in meaning as well as in name.
- The post has a new filename, and Fusion identifies a post by filename. Remove
MPCNC_v4.0_Beta2.cpsfrom the Post Library rather than leaving it beside Beta 3.
→ Full release notes for Beta 3 — what changed, per firmware, and what is not verified.
Beta 1 knew one zero: wherever the tool happened to be when the job started. Beta 2 keeps track of one per part, plus one job-level height in the machine's own frame to cross the bed at.
- More than one work zero. Beta 1 set a single origin for the whole program. Beta 2 stores a
separate zero for each part, in the controller's own registers, and switches between them as
the job runs. All three firmwares have those registers; on Marlin they arrive with one build
option (
CNC_COORDINATE_SYSTEMS), which the post assumes and warns about rather than refusing. → What a work offset is - You choose how each zero gets set. Beta 1 had two checkboxes. Beta 2 asks you to pick: use where the tool is now, use a zero the controller already has stored, or stop and let you jog to it — each with or without probing Z off a touch plate. → Origin modes in full
- Several parts in one job. Parts on separate fixtures cut in a single run, re-probing each one so stock thickness can vary — and one part from several datums on one fixture, each datum being a work offset like a part. → Several parts in one job
- The machine frame, split in two. Group 4 separates what your machine can home from what this job should do about it, so "homed at the controller, do not home here" is now sayable. → The machine frame
- One travel height in the machine's own frame. Machine Travel Z is an absolute machine coordinate, read off your sender once and typed in. The machine's homed Z is the only frame whose Z0 does not move with stock thickness, so it is the only height that can clear every fixture on a job whose parts differ in thickness — and a multi-part job is refused without it. → The travel height
- Tool changes rebuilt around what the post can actually do, which is arrive, hand over and resume. Group 6 asks who performs the change — nobody (refuse the job), you at a pause, or your sender's or firmware's own macro — and, separately, who corrects Z0 for the new tool's length. A multi-tool job is now refused by default rather than posted with its changes silently dropped. → Tool changes
- Unsafe jobs are refused before any file is written, with a message saying what to change; many more conditions warn you — in Fusion's post dialog, in the file, or in both. → Validation guards
- Better probing. Prompts to attach and remove the probe, and the option to touch off away from the part origin so that origin can sit off the material. → Probing
- The dialog was rebuilt — 10 numbered groups in the order you work through them, and every setting is dumped at the head of the posted file, together with the values the post resolved from them. → Property reference
- Safer endings and clearer prompts. The spindle stops before the tool parks; a hand-set router is prompted whenever the speed or direction changes, not only at the start; and each firmware gets the right end-of-program code.
- Saved settings do not carry over from Beta 1, and several were rebuilt during the Beta 2 series itself — the dialog's internal keys changed, so expect to re-enter a customised preset once. Check groups 4, 5 and 6 before your first job: the origin choice is new and its default is not what Beta 1 did, Machine Travel Z ships empty on purpose, and At a Tool Change ships at Refuse a multi-tool job. Scale Feedrate is now on, and the coolant channel codes default to the GRBL dialect rather than Marlin's.
Beta 1 was v3.0 Beta 3 renamed — the post itself was unchanged. Its work was tidying and correctness rather than new machine features:
- A grouped, named property dialog in place of a flat list of settings.
- Drilling operations post at all — canned cycles are expanded into ordinary moves.
- Manual NC pass-through commands are emitted as written.
- Rapid moves are ordered so the tool lifts before it travels and travels before it descends, instead of dragging or plunging.
- Jobs the post can't handle are refused with a useful message — 4/5-axis toolpaths, and cutter compensation set to anything but In computer.
- A long list of smaller corrections.
- Only 3-axis toolpaths — 4/5-axis operations error out.
- Cutter/radius compensation must be In computer; control-side G41/G42 is a posting error.
- A Setup built on a tilted face is refused, with the tilt named — the tool only moves straight down, so a Setup whose Z is not the machine's Z would cut in the wrong plane.
- CAM probing operations are refused. The post's own Z touch-off is not one of them; a Fusion WCS-probing operation asks the controller to measure and store an offset, which none of these controllers can do.
- Arcs are on the XY plane (Marlin/RepRap) or all planes (GRBL); full circles post as two arcs; helical moves are linearised.
- Canned cycles (drill/peck/bore/tap) are expanded into plain G0/G1/G4 moves. No supported firmware has them — and on RepRap those g-code numbers mean bed probing instead, which is worse than absent.
- Manual NC Pass through commands are emitted verbatim.
M1(optional stop) is emitted asM0. No supported firmware gives the optional half a usable meaning: GRBL parsesM1and does nothing, RepRap treats it as end-of-job, and only Marlin waits for the LCD. The file says so where it happens.- Travel Speed X/Y and Travel Speed Z do nothing on GRBL or FluidNC. Their planner takes a
rapid's rate from the axis maximums held in the controller, not from the
Fword in the block, and no line a posted file may contain changes that. Marlin and RepRap obey both. - End of program differs by firmware. GRBL ends with
M30. Marlin and RepRap getM84 S60first, restoring the 60-second idle timeout the post disables for the duration of the job (a bareM84would drop an unbalanced gantry in Z). RepRap then getsM2, which it has supported since RRF 3.5.1 and which runs yourstop.g— if that macro disables the steppers, it overrides the timeout just set. Marlin gets no program-end code because it has never implemented one:M2is unknown there andM30means "delete SD file", so on Marlin the end of the file is the end of the program. - No
%wrapper is written, on any firmware — stock Grbl 1.1 has no%feature, so the line reaches the parser and answerserror:1. - GRBL laser jobs likely need laser mode enabled
(
$32=1). - Firmware claims in these documents are settled from each firmware's own source and changelog, with the file and version cited. This project has no controller to test against, so nothing here is proved by having been run on a machine — see what is verified.