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) post processor, distributed as the single file
MPCNC_v4.0_Beta2.cps.
Supported firmware (set by the Job → CNC Firmware property):
- GRBL 1.1 / FluidNC
- Marlin 2.x
- RepRap firmware (Duet3D)
- Repetier 1.0.3 (untested; g-code is the same as Marlin)
Beta 1 knew one zero: wherever the tool happened to be when the job started. Beta 2 can keep track of several — the machine, the spoilboard, and each part — and move safely between them.
- More than one work zero. Beta 1 set a single origin for the whole program. Beta 2 can store a separate zero for each part, in the controller's own memory, and switch between them as the job runs. (Marlin can still only hold one.) → What is a WCS?
- You choose how the 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
- Several parts in one job. Cut copies of a part on separate fixtures in a single run, re-probing each one so stock thickness can vary. → Multiple fixtures
- Homing at job start, if your machine has endstops — new group 04. → Establishing the machine frame
- A spoilboard reference — new group 05. Zero one slot to the table rather than to the stock, so the tool can lift to a height that clears everything on the bed before it travels to another part. → The reserved spoilboard base
- Unsafe jobs are refused before any file is written, with a message saying what to change, and two common mistakes now warn you. → Validation guards
- Better probing. Prompts to attach and remove the probe, and the option to touch off away from the corner so the origin can sit off the material. → Probing and tool changes
- The dialog was rebuilt — 11 groups instead of 9, numbered in the order you work through them, and every setting is now listed at the top of the posted file. → Property reference
- Safer endings and clearer prompts. The spindle stops before the tool returns to X0 Y0; a hand-set router is prompted whenever the speed or direction changes, not just at the start; and each firmware now gets the right end-of-program code.
- Your saved settings carry over, but check group 06 before your first job — the origin choice is new and its default is not what Beta 1 did. One setting does need changing: the coolant "… Custom" boxes now want a filename, not g-code. → 10 - Coolant
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.
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, 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 is used for X/Y repeatability, never as the everyday Z reference.
The post is designed to degrade gracefully:
- A hobby job — one operation, one part — needs almost no setup. Jog to your zero, accept the defaults (the post records XY there and probes Z for you), post, run.
- A full job — many operations, multiple tools, or multiple fixtures making several copies — has the extra structure (WCS handling, a reserved spoilboard base, per-part probing, safe cross-part traverses) 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; adjustable comment verbosity; 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 all post properties must be entered in millimeters.
The post is a single file, MPCNC_v4.0_Beta2.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.
- Use the Import icon to import
MPCNC_v4.0_Beta2.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.
Who this is: you're cutting one part in one Setup containing one Operation, with a single tool, and zeroing by hand before posting the job to your CNC. A single operation has no WCS change, so only the First WCS / Part origin choice applies.
Review the property groups in the dialog from top to bottom.
Only three groups need any attention for users running the hobbyist limited version of Fusion 360; for the rest you may just Accept the Defaults.
The groups are ordered to be worked through in sequence. Groups 01–03 describe your machine and how it should move; groups 04–06 — Establish Machine Coordinates, Establish Spoilboard Reference, On WCS / Part / Fixture Changes — decide where things are, and are listed in the order the machine does them: find the machine's own zero, then the spoilboard, then each part. Groups 07–11 are optional hardware and add-ons.
- 01 - Job
- set CNC Firmware to your controller.
- Leave Manual Spindle On/Off on if you start your router/spindle by hand.
- Other fields Accept Defaults.
- 02 - Feeds and Speeds
- set Travel Speed X/Y, Travel Speed Z, and the Max XY Cut Speed / Max Z Cut Speed limits to your machine's real capability.
- Enable Scale Feedrate so cut moves are scaled to stay within those limits, and keep Enforce Feedrate on so a feedrate is always included on each gcode statement.
- 03 - Map G1s to Rapids - disable when using full license
- Hobbyists should turn all options in this group on.
- A Personal-license of Fusion 360 forces all rapid moves to be emitted as cutting moves.
- Converts some of the cutting movements back to rapids and restores safe, properly-ordered travel moves (retract before travelling, travel before descending) and avoids dragging the tool across the work. (See G1 → G0 rapid mapping.)
- 04 - Establish Machine Coordinates
- Accept Defaults (Home Before Start = None).
- Choose XY only if your machine has X/Y endstops and you want squaring included in the post.
- 05 - Establish Spoilboard Reference
- Accept Defaults (Reserved WCS = None).
- Understanding the true zero height of the spoilboard is only important during multi-part moves, not an option in the hobbyist version.
- A single-part job requires no base.
- 06 - On WCS / Part / Fixture Changes
- Accept Defaults.
- First WCS / Part defaults to
Set X0 Y0 to Current Pos, Probe Z0- Before sending your post to the CNC, jog the tool to the part's XY corner (in your sender).
- The post records the current XY and then probes Z off a touch plate.
- Optional: use the X Y probe offset to offset the probing operation.
- Keep Probe Pause = Before & After so you're prompted to attach/remove the probe.
- If you have no probe on your CNC, choose
Set X0 Y0 Z0 to Current Posinstead.- Jog your CNC to XY and touch Z before posting job to CNC.
- Prefer a guided jog prompt?
- The
Jog to …modes pause mid-run and ask you to jog to the origin instead of pre-jogging. They are not the default because jogging while paused isn't supported on every firmware/sender — see Jogging at a pause.
- The
- 07 - Tool Changes
- Accept Defaults. (Tool Changes are Included = Off)
- 08 - External Include Files
- Accept Defaults. (All Empty)
- 09 - Laser
- Accept defaults unless this is a laser job.
- 10 - Coolant
- Accept Defaults unless CNC has coolant hardware.
- 11 - Duet
- Accept Defaults unless running Duet firmware.
- Built-in
- Consult Fusion 360 documentation before changing.
Then select post.
A Work Coordinate System (WCS) is a stored origin the controller remembers.
On GRBL and RepRap there are several — G54, G55, G56, G57, G58, G59 (and
G59.1–G59.3 on RepRap only). Selecting one (e.g. G54) tells the controller "from
now on, X0 Y0 Z0 means this stored position on the CNC." Each WCS holds its own offset, so you can
define several independent zeros and switch between them mid-program without disturbing
the others.
Only a full-license user has the option of utilizing WCSs.
Multiple WCS are commonly used when multiple parts are being milled at different positions (fixtures) on the CNC. The 0,0 origin of each fixture is set into sequential WCSs prior to posting the job.
Fusion assigns a WCS to each Setup via its Work Offset field (1 → G54, 2 → G55,
…). This post emits the matching WCS when it changes in Fusion.
Marlin firmware is an exception. Marlin has no work-offset table — it has a single global origin set with
G92. So on Marlin only one coordinate frame exists; a job that uses more than one distinct work offset is rejected at the time the post processor is run (see Validation guards). Everything below about multiple WCS applies to GRBL and RepRap.
The common full-license job: several operations (face, pocket, contour), possibly several tools, all on one part in one Setup — so one WCS throughout.
- Turn the 03 - Map G1s to Rapids - disable when using full license group off — the
full license already posts real
G0rapids, so the hobby workaround isn't needed. - Set First WCS / Part:
- If this Setup's WCS is a pre-set fixture, choose
Use Active WCS X0 Y0, Probe Z0(rapid to the stored X0 Y0, re-probe Z); - Otherwise
Set X0 Y0 to Current Pos, Probe Z0(pre-jog XY). - Prefer these methods over the
Jogmodes.
- If this Setup's WCS is a pre-set fixture, choose
- If the job changes tools, enable the 07 - Tool Changes group.
- Because there is no tool-length system, turn on Probe After Tool Change so each new tool re-references Z.
- The tool-change park position (Tool Change X/Y/Z) is relative to the current work zero.
- EXPECT ENHANCEMENTS TO TOOL CHANGES in future updates.
- One WCS means one shared frame, so each operation's own retract moves already clear the part. Since there are no cross-part / cross-WCS moves, there is no need to establish a Spoilboard Reference.
You have jigged up several copies of the same part, one per fixture, each on its own
WCS (G54, G55, G56, …), and want to cut them all in one program.
- Reserve a spoilboard base
- Set 05 - Establish Spoilboard Reference → Reserved WCS (recommended
G59).- This is a fixed-surface zero (the spoilboard, not any stock top) that gives the post a stable reference to retract to when traversing between parts of possibly different thickness.
- Keep Probe to Set Base at
Pause, Probe Z, Pause(orProbe Zif pausing to probe is not required). - Probing the spoilboard will occur at the current CNC's position. No XY movement will occur prior to the probe.
- The Reserved WCS will be utilized to record the Z0 of the spoilboard.
- Attempts to change the Reserved WCS Z0 with an operation will cause a post error. Keep the reserved base as the fixed spoilboard reference. A guard trips only if an operation would re-establish the base's origin (re-zero or re-probe it); it doesn't otherwise stop you from selecting that WCS for an operation.
- Set 05 - Establish Spoilboard Reference → Reserved WCS (recommended
- Put each copy on its own Fusion Work Offset.
- Their XY comes from each fixture's
pre-set offset
- The post never sets XY for an added part unless you choose a Jog mode.
- Their XY comes from each fixture's
pre-set offset
- The first copy uses First WCS / Part
- Choose
Use Active WCS X0 Y0, Probe Z0so it too takes its pre-set XY and re-probes Z (matching the copies below).
- Choose
- Subsequent WCS / Part decides what happens at each copy after the first.
- Best-practice paths use the stored fixture offset — not jogging
- Use Active WCS X0 Y0, Probe Z0 (default)
- Rapids to that copy's stored X0 Y0 and re-probes its stock-top Z.
- Handles varying stock thickness.
- Use Active WCS X0 Y0 Z0
- The copy uses whatever X0 Y0 Z0 is already stored in the corresponding WCS; the tool just rapids there (no probe).
- Jog to X0 Y0, Probe Z0 / Jog to X0 Y0 Z0
- Pause (
M0) so the operator can jog to each copy's origin. - Only for a setup run where the fixtures are not pre-set, and only if your firmware/sender supports jogging during a pause (see Jogging at a pause).
- Pause (
- Retract Across Parts (on by default)
- Makes the tool retract to Inter Part Safe Z — an absolute height above the spoilboard base — before it traverses to the next fixture, so it clears every clamp and part regardless of their heights.
Reestablishing the same part for a second reference, or flipping it, is out of scope for a single post run. On a machine with no homing the post cannot establish the second reference's XY, and re-probing the same surface buys nothing. Run each reference / each side as a separate job. Future enhancements may add additional functionality.
Production controls keep three references separate: the machine frame (G53, from
homing), the work frame (G54–G59), and tool-length offsets (TLO, G43, from a tool
setter). Most V1E machines have none of the three fully, so this post takes a deliberate
work-relative stance:
- The everyday reference is the active WCS, not the machine frame.
- Tool length is folded into a Z re-probe after each tool change — there is no TLO.
- Homing establishes the machine frame for X/Y only (squaring and a repeatable origin), as an optional robustness feature. Z homing, where it exists, is for its own sake (a real endstop, or the movable-plate trick) and never becomes the everyday Z reference — that is always the work-Z touch-off.
This matches the GRBL ecosystem (Shapeoko / OpenBuilds / Onefinity all zero to the work and probe Z) and works on the lowest-common-denominator machine.
Group 06 - On WCS / Part / Fixture Changes holds the two origin controls. Each is an explicit taxonomy with three families:
- Set … to Current Pos — no prompt. The tool is assumed to already be at the origin (you pre-jogged before starting, or machine homing / the spoilboard base left it there); the post records the current position. (First WCS / Part only.)
- Use Active WCS … — no prompt. Trust the origin already stored in that WCS (a
pre-set fixture offset / a prior job): rapid to its stored X0 Y0, and either re-probe Z
(
… X0 Y0, Probe Z0) or trust the stored Z too (… X0 Y0 Z0, no probe). The best-practice path for pre-set fixtures. See What "Active WCS" means below — it is not whatever WCS your sender currently has selected. - Jog to … — the post pauses with an
M0(or RepRapM291) so the operator jogs to the origin during the run, then records it there.
Each probe family comes in a Z-manual variant (… X0 Y0 Z0, no probe) and a
probe-Z variant (… X0 Y0, Probe Z0). On a jet tool or tool 0 the probe is skipped
automatically. The defaults avoid any run-time jog pause (which not every
firmware/sender supports — see Jogging at a pause): First WCS / Part defaults to
Set X0 Y0 to Current Pos, Probe Z0 (pre-jog XY in your sender, then probe Z), and
Subsequent WCS / Part to Use Active WCS X0 Y0, Probe Z0 (pre-set fixture XY,
re-probe Z). Pick a Jog to … mode only when you want the post to pause and guide you
and your setup supports jogging at the pause.
A jet tool or tool 0 never probes. Any probe-Z mode degrades to recording the origin with no
G38.2, on every firmware. On a probe-Z mode that also means Z0 is never established — the job then runs against whatever Z origin the register already holds, so the post emits a warning. For a laser / jet job chooseSet X0 Y0 Z0 to Current Posand set Z by hand.
⚠
Use Active WCS X0 Y0 Z0starts by moving Z to Safe Z, then rapids to the stored X0 Y0. Safe Z is an absolute height in the stored frame, so this is a retract only if the tool is below it — park the tool above Safe Z and the job's first motion is a descent, at Z travel speed, over ground the post knows nothing about. The post cannot do better: it has no way to read the physical Z, and the premise of the mode is that the stored frame is trusted. Either park below Safe Z, or raise Safe Z (group 06) to clear everything.
The WCS your Fusion Setup designates — not the one your sender happens to have selected. Worth being precise about, because the two are easy to conflate:
- Each Fusion Setup carries a Work Offset (its WCS). That is what the post uses:
G54unless you set it to something else, and one WCS per part in a multi-part job. - The post selects that WCS itself, at job start, before it establishes any origin. So if
you left
G55active in your sender and this Setup says WCS 1, the file emitsG54and the job runs there regardless. The post overwrites the selection — it never inherits it. You do not need to pre-select a WCS in your sender. - What the post cannot do is read that WCS's stored origin. Register contents are runtime state in the controller (GRBL keeps them through a power cycle), written by a previous job or by your own manual touch-off. A post is a one-way g-code generator — there is no round trip.
So the split is: which WCS is certain; what it contains is trusted. That is exactly what the
Use Active WCS … modes assume, and why they are the right choice only when you know the stored
origin is still good:
| Safe to use | Watch out for | |
|---|---|---|
Use Active WCS X0 Y0, Probe Z0 |
XY fixtures are pre-set and unchanged; stock thickness may vary (Z is re-probed) | A fixture that moved — XY is trusted blindly |
Use Active WCS X0 Y0 Z0 |
Nothing has changed since the origin was set, incl. stock thickness | New/different stock — the stored Z will be wrong; and the opening move to Safe Z can descend (above) |
On a fresh controller every offset is 0, so G54 means machine coordinates — on a machine
with no endstops, wherever it powered on. Don't use a Use Active WCS … mode until the WCS has
actually been set (by a prior run, or by hand). The Set … to Current Pos and Jog to … families
establish the origin instead of relying on one, which is why one of them is the default.
The Jog origin modes (and the pre-homing prompt) pause the program and expect you to jog the tool by hand, then resume. Whether you can actually jog while paused depends on your firmware and sender:
- RepRap / Duet — fully supported by design. The post emits
M291 … S3 X1 Y1 Z1, a blocking dialog with on-screen jog buttons for X/Y/Z. - GRBL / FluidNC — the post emits a plain
M0pause; whether you can jog then is a property of your sender, not the firmware. CNCjs, UGS, and bCNC keep GRBL in Idle at the pause and let you jog, then resume with cycle-start; a bare-bones sender may hold GRBL in a state that refuses$J=until you resume. - Marlin — jog from the LCD/controller (Move-Axis menu) while paused at the
M0. Host-streamed jog moves would just queue behind the pause and not run until you resume.
Group 04 - Establish Machine Coordinates → Home Before Start decides whether the machine homes at job start to establish a repeatable machine frame:
- None (default) — emit no homing; accept the current position (already homed at the
controller, or a power-on
0,0,0). The safe default — a wrong home command is a crash. - XY — home X and Y (the usual case: XY repeatability and gantry squaring; Z stays on the work-Z probe touch-off).
- XYZ — also home Z, only if the machine is actually wired to home Z (LowRider switches, or the Marlin movable-plate trick).
Homing command by firmware:
| Firmware | Command |
|---|---|
| Marlin / RRF (Duet) | G28 X / G28 Y / G28 Z — each axis homed independently |
| GRBL / FluidNC | $H only — one command homes all configured axes together |
On GRBL/FluidNC $H is all-or-nothing, so XY and XYZ emit the same $H (the
choice just documents intent). Prompt Before Home pauses before homing so you can
prepare the machine (place a movable Z plate, clear the bed); it fires whenever homing
runs, so it never needs revisiting when the machine changes.
For multi-fixture jobs, one WCS can be reserved as a spoilboard base (05 - Establish
Spoilboard Reference → Reserved WCS, default None). Because it is zeroed to a fixed
surface (the spoilboard, independent of stock thickness), it is the one frame in which a
safe height is meaningful across all of a job's parts. It is:
- Established at job start by Probe to Set Base:
Pause, Probe Z, Pause(prompt, probe, prompt — the manual touch-off, default),Probe Z(probe with no prompt, a fixed point), orNone(assume pre-set from a prior job — probe once, run many).⚠ Park over bare spoilboard before you start. The base probe makes no XY move — it touches off whatever is under the tool at job start. Park over the stock and the "spoilboard base" silently records the stock top instead, and every clearance measured from it is short by the stock thickness. The Probe X/Y Offset shifts only part probes and cannot be used to move this one.
- Transited, not parked: when the tool must move between parts, the post briefly selects the base to retract to Inter Part Safe Z (the group's cross-part clearance), then selects the destination WCS. It never leaves the base active into a cut, and never selects it without a real move.
- Recommended slot
G59(the highest GRBL supports, keepingG54free for parts).G59.1–G59.3are RepRap-only; a base is ignored on Marlin.
- Work-Z probing only.
G38.2down to a touch plate (thickness compensated via Plate Thickness), with attach/remove pauses governed by Probe Pause. There is no tool-length system, and X/Y is never probed (jog manually). - G38 Target is a travel limit, not a destination — on the modes where the post can make it
one.
G38 Targetis emitted as aZword, so it means "descend to this height in the current work frame". On the two modes where you have just placed the tool — Set X0 Y0 to Current Pos, Probe Z0 and Jog to X0 Y0, Probe Z0 — the post writes a provisionalZ0at the current height before probing, so the default-10really is "descend at most 10 mm" and the probe overwrites it moments later. On the Use Active WCS … and added-part modes it cannot: the tool arrives from a retracted clearance, so the target stays relative to the stored zero. Size it against that stored zero on those modes, or the probe can run long or never contact at all. - Probe Pause (default
Before & After) controls the operator prompts around each part probe — attach before, detach after; setNofor a fixed/permanent probe. It does not affect the spoilboard base probe (see Probe to Set Base). - Probe X/Y Offset (default
0,0) moves the Z-probe touch-point away from the work origin by a fixed XY distance, so the origin can sit at a part corner or off the material while Z is still read on the stock top. It applies at every part probe — the first part and each added copy — and is job-wide, not per-fixture. It never applies to the spoilboard base probe, which makes no XY move at all (see The reserved spoilboard base). - Re-probe after every tool change is the tool-length substitute — enable Probe After Tool Change.
- Manual tool changes (no ATC): retract, move to the work-relative change position, pause for the swap, re-probe Z, resume. Every leg is collision-sensitive.
With Manual Spindle On/Off on (the default) the post never emits M3/M5. Instead it
stops the machine and asks you, so a hand-switched router or trim spindle is safe:
- At job start —
Turn ON 7000 RPM(the direction is named only when the operation is counterclockwise, which is the exceptional case). - Whenever the speed or the direction changes —
Set spindle to 10000 RPM clockwise. A change prompt always states the full target, so there is nothing to remember. A second operation at a different RPM, and a tapping reversal, both trip this. - At each tool change and at the end of the job — a prompt to switch off. At the end this comes before the return to X0 Y0, so you switch off, resume, and the machine parks.
Turn the property off if your spindle is under g-code control; you then get real
M3 S…/M5 and no prompts.
Group 08 - External Include Files lets you substitute your own g-code, read from a file in the nc output folder, at five points in the program.
An include file replaces the phase it names — it does not add to it. That is the point of the feature, but it means the built-in code for that phase, including the modal preamble, is not emitted:
- A Start GCode File owns
G90andG21/G20, plusG94andG17on GRBL, or theM84 S0stepper-timeout disable on Marlin/RepRap. Your file must set whatever it needs.- A Stop GCode File owns coolant-off, the spindle-off prompt, the At End Go to 0,0 move,
M84 S60, andM30/M2. (On GRBL the closing%is still written.)- A file that exists but is empty is the same rule taken to its limit: the phase is still replaced, by nothing. The post says so with an Info comment rather than leaving you to wonder.
- A file that is named but missing aborts the post with an error.
Fusion will ask "This post processor might be unsafe…" the first time you name any file here — reading a file is what triggers it. Answer Yes; answering No cancels the post.
Tool Change Probe is not implemented. The field exists and is reserved, but nothing reads it — anything typed there is ignored, silently. Its title says so.
The post checks the job at post time (it can't read the live controller) and errors before emitting bad g-code:
- No base redefine — using the reserved base is fine; a job that would re-establish its origin is an error ("assign this operation to another WCS").
- Safe-Z across parts needs a base — if Retract Across Parts is on and the job uses more than one WCS on GRBL/RRF with no base reserved, it errors (a clearance height is meaningless across un-probed offsets). Single-WCS jobs are exempt.
- Marlin is single-frame — a Marlin job that uses more than one distinct work offset
is a hard error (
G92can't fake multiple WCS). - The tool axis must be machine +Z — a 3-axis Setup built off a model face rather than the stock top posts geometry the machine would cut in the wrong plane, so an off-axis section is rejected with the tilt named. Re-orient the Setup's Z. Unlike the guards above this one fires once output has started, so it leaves a truncated file on disk; discard it.
Two further checks warn rather than stop the post — each is legitimate on some setup, so you are told, not blocked. The message appears in Fusion's post dialog:
- Homing plus a
Set … to Current Posorigin mode. Homing runs first and parks the tool at the endstop corner, so the origin is recorded there and the pre-jog you did is discarded. Choose aUse Active WCS …orJog to …mode, or set Home Before Start toNone. Legitimate only on a machine whose home corner is the datum. - More than one tool with Tool Changes are Included off. No tool-change code is emitted, so every operation runs with whichever tool is already in the spindle, at the other tools' feeds and speeds. Enable group 07, or post one tool per file. The file also marks each suppressed change.
A third warning is written into the file rather than the dialog: a jet / laser tool cannot probe, so on a probe-Z origin mode Z0 is never established and the job runs against whatever Z the register already holds.
The Personal license restricts all moves to the max cut speed — and Fusion implements
this by turning every G0 rapid into a G1 cut. The side effect is dragging cuts and
collisions at the start of jobs and after tool changes. Group 03 - Map G1s to Rapids -
disable when using full license selectively converts those G1 moves back into G0
rapids where it's safe:
- First G1 → G0 Rapid — restores the lost initial positioning move at the start of a toolpath (the "tool dragged across the work" problem).
- Map: G1s → G0 Rapids — converts horizontal
G1moves at or above Map: Safe Z to Rapid into rapids (assumes anything at that height is a safe air move). - Map: Safe Z to Rapid — the Z height where a cut move will be considered safe to convert
to a rapid. Defined as a Fusion layer followed by a fallback constant used when the layer is not defined
(eg
Retract:15,Feed:5,Clearance:7). - Map: Allow Rapid Z — also convert safe vertical moves.
The post emits rapid G0 moves as two moves — Z and XY separately, ordered so the tool
retracts before travelling and travels before descending — which is what makes these
conversions safe. A true cutting move is never converted. Full-license users disable this
whole group — Fusion 360 will post true rapid G0 and G1 cutting moves — enabling will corrupt
Full-license posts.
Travel Speed X/Y and Travel Speed Z are always used for G0 rapids. If Scale
Feedrate is on, G1 cut feedrates are scaled so no axis exceeds its Max XY / Max Z
Cut Speed: the toolpath feed is projected onto each axis, over-limit axes are scaled
down proportionally, and the result is capped at Max Toolpath Speed. Scaling only
ever reduces a feed. (Because scaling is 3-dimensional, a resulting toolpath feed can
look higher than a single axis limit while each axis is still within its own limit.)
G2/G3 arcs are scaled too, against the limits of the plane the arc lies in — an XY arc
against Max XY Cut Speed, a ZX or YZ arc against the slower of the two axes it sweeps. An arc
can therefore post slower than the straight moves either side of it and still be right: a
diagonal G1 splits its feed across two axes, while an arc reaches the full feed on one axis at
each quadrant, so the post holds it to the axis limit.
Groups appear in the Fusion dialog in the order below.
| Title | Description | Default |
|---|---|---|
| CNC Firmware | Dialect of g-code to create (GRBL / Marlin / RepRap). | GRBL |
| Manual Spindle On/Off | Issue pauses to manually turn the spindle on/off — a prompt to switch on at the start, to change speed or direction whenever the job asks for a different one, and to switch off at each tool change and at the end, on every firmware. No M3/M5 is emitted on this path; the post asks rather than commands. See Manual spindle control. |
true |
| Comment Level | Verbosity: Off, Important, Info, Debug. | Info |
| Use Arcs | Use G2/G3 for circular moves. | true |
| Enable Line #s | Emit sequence numbers. | false |
| First Line # | First sequence number. | 10 |
| Line # Increment | Sequence-number increment. | 1 |
| Include Whitespace | Whitespace separation between words. | true |
| At End Go to 0,0 | Go to X0 Y0 at program end; Z unchanged. The spindle is stopped (or the switch-off prompt issued) before this move. | true |
| Title | Description | Default |
|---|---|---|
| Travel Speed X/Y | G0 travel speed X & Y (mm/min). |
2500 |
| Travel Speed Z | G0 travel speed Z (mm/min). |
300 |
| Enforce Feedrate | Always emit Fxxx even when unchanged (useful for Marlin). |
true |
| Scale Feedrate | Scale G1 feeds to axis maximums. |
false |
| Max XY Cut Speed | Max X or Y cut speed (mm/min). | 900 |
| Max Z Cut Speed | Max Z cut speed (mm/min). | 180 |
| Max Toolpath Speed | Cap for the scaled toolpath feed (mm/min). | 1000 |
| Title | Description | Default |
|---|---|---|
| First G1 → G0 Rapid | Convert the first G1 of a toolpath to a rapid. |
false |
| Map: G1s → G0 Rapids | Convert safe horizontal G1 moves to rapids. |
false |
| Map: Safe Z to Rapid | Threshold Z: a number, or a Fusion height with fallback (e.g. Retract:15). |
Retract:15 |
| Map: Allow Rapid Z | Also convert safe vertical moves. | false |
| Title | Description | Default |
|---|---|---|
| Home Before Start | Home at job start to establish the machine frame: None (no homing), XY (home X/Y), XYZ (also home Z, only if wired for it). GRBL homes all axes with one $H if XY or XYZ. Warns if combined with a Set … to Current Pos origin mode — homing would overwrite your pre-jog. |
None |
| Prompt Before Home | Pause before homing so you can prepare the machine (place a movable Z plate, clear the bed). Fires whenever homing runs. | false |
| Title | Description | Default |
|---|---|---|
| Reserved WCS | Reserve one WCS as a fixed spoilboard base. None = off. G59.1–G59.3 are RepRap-only; ignored on Marlin. |
None |
| Probe to Set Base | Set the base's Z at job start: None (assume pre-set), Probe Z (probe, no prompt), Pause, Probe Z, Pause (manual touch-off). Probes wherever the tool is parked — no XY move is made and Probe X/Y Offset never applies, so park over bare spoilboard. | Pause, Probe Z, Pause |
| Retract Across Parts | Retract to Inter Part Safe Z (below) before traversing between WCS; drives the safe-Z guard. GRBL/RepRap only. | true |
| Inter Part Safe Z | Absolute height above the base to retract to between parts — clear the tallest fixture. | 40 |
| Title | Description | Default |
|---|---|---|
| First WCS / Part | Origin for the first/only part: Set X0 Y0 to Current Pos, Probe Z0 / Set X0 Y0 Z0 to Current Pos / Use Active WCS X0 Y0, Probe Z0 / Use Active WCS X0 Y0 Z0 / Jog to X0 Y0, Probe Z0 / Jog to X0 Y0 Z0. Use Active WCS X0 Y0 Z0 opens with a move to Safe Z that can descend — see Origin modes. |
Set X0 Y0 to Current Pos, Probe Z0 |
| Subsequent WCS / Part | Multi-part only — what to do at each added part's WCS: Use Active WCS X0 Y0, Probe Z0 / Use Active WCS X0 Y0 Z0 / Jog to X0 Y0, Probe Z0 / Jog to X0 Y0 Z0. Not supported on Marlin. | Use Active WCS X0 Y0, Probe Z0 |
| Probe Pause | Operator prompts around each part probe: No / Before / Before & After. | Before & After |
| Probe X Offset | X from a part's origin to its Z-probe touch-point. Applied at every part probe (first + added), never to the spoilboard base probe. 0 = probe at the origin. |
0 |
| Probe Y Offset | Y from a part's origin to its Z-probe touch-point. Applied at every part probe (first + added), never to the spoilboard base probe. 0 = probe at the origin. |
0 |
| Probe with G38.2 | Probe with G38.2 (On) or G28 (Off). GRBL always G38.2. |
On |
| G38 Target | Furthest Z the probe move travels to. A true relative limit on the two just-positioned modes; relative to the stored zero on the Use Active WCS … modes — see Probing and tool changes. | -10 |
| G38 Speed | Probe feedrate (mm/min). | 30 |
| Safe Z | Retract height after probing; the no-base added-part re-probe retract; and the height Use Active WCS X0 Y0 Z0 moves to before rapiding to the stored X0 Y0. A number or a Fusion height (e.g. Retract:15). |
Retract:15 |
| Plate Thickness | Touch-plate thickness (compensated into Z). | 0.8 |
| Title | Description | Default |
|---|---|---|
| Tool Changes are Included | Emit tool-change code when the tool changes. Left off in a multi-tool job the post warns, and each suppressed change is marked in the file. | false |
| Include Relocation Code | Move to the change position (X/Y/Z below); off = plain M6/select. | false |
| Tool Change X / Y / Z | Change position, relative to the current WCS (plain G0). |
0 / 0 / 40 |
| Disable Z Stepper | Disable the Z stepper after reaching the change position. | false |
| Do First Change | Do an initial change to load the first tool. | false |
| Probe After Tool Change | Re-probe Z after each change (the tool-length substitute). | false |
Each names a file in the nc output folder whose contents are inserted verbatim at that point. Leave empty for built-in code. A Start or Stop file replaces that phase, modal preamble and all — see External include files. Naming any file here makes Fusion ask "This post processor might be unsafe…"; answer Yes.
| Title | Description | Default |
|---|---|---|
| Start GCode File | Replaces the whole start phase — your file owns G90, G21/G20, and G94/G17 (GRBL) or M84 S0 (Marlin/RepRap). |
empty |
| Stop GCode File | Replaces the whole stop phase — your file owns coolant-off, the spindle-off prompt, the At End Go to 0,0 move, M84 S60 and M30/M2. |
empty |
| Tool Change Start / Tool Change End | Inserted around the tool-change code (added, not substituted). | empty |
| Tool Change Probe | NOT IMPLEMENTED. Reserved; anything entered is ignored with no warning. | empty |
Fusion's four Through levels all map to "On - Through". The CNC Firmware selection decides whether the GRBL or Marlin/RepRap laser mode is used.
| Title | Description | Default |
|---|---|---|
| Laser: On - Vaporize / Through / Etch | Power % per cutting mode. | 100 / 80 / 40 |
| Laser: Marlin/Reprap Mode | Fan (M106/M107), Spindle (M3/M5), or Pin (M42). | Fan - M106 S{PWM}/M107 |
| Laser: Marlin M42 Pin | Custom pin for Pin mode. | 4 |
| Laser: GRBL Mode | Dynamic (M4) or static (M3) power. | M4 S{PWM}/M5 dynamic |
| Laser: Coolant | Force a coolant for laser ops (e.g. air). | Off |
Two channels (A, B); each maps a Fusion coolant mode to enable/disable g-code. If a tool's coolant matches a channel, that channel is enabled; a warning is emitted if a requested coolant matches no channel. Marlin and GRBL command options are both offered — pick to match your wiring.
For anything the built-in options don't cover, set Turn Channel A/B On (or Off) to
Use custom and put the name of a file in the matching … Custom field — these name a
file in the nc output folder exactly as the group-08 include fields do, not a literal g-code
block. The file's contents are inserted at that point; a missing file aborts the post, and
Use custom with the field left empty emits a warning and nothing else. As with group 08,
Fusion asks "This post processor might be unsafe…" the first time — answer Yes.
| Title | Description | Default |
|---|---|---|
| Channel A / B Mode | Coolant mode that enables the channel. | off |
| Turn Channel A / B On/Off | Enable/disable g-code for the channel, or Use custom. | M42 P6/P11 S255/S0 |
| Channel A / B On/Off Custom | Filename (in the nc folder) included when the matching On/Off is set to Use custom. |
empty |
| Title | Description | Default |
|---|---|---|
| Milling Mode | Duet3D milling-mode command. | M453 P2 I0 R30000 F200 |
| Laser Mode | Duet3D laser-mode command. | M452 P2 I0 R255 F200 |
- 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.
- Arcs are on the XY plane (Marlin/RepRap) or all planes (GRBL); full circles are two arcs.
- Canned cycles (drill/peck/bore/tap) are expanded into plain G0/G1 moves.
- Manual NC Pass through commands are emitted verbatim.
- 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. - GRBL laser jobs likely need laser mode enabled
(
$32=1). - Built-in tool change with LCD/SD: printing from SD and using the LCD to restart is required.