Overview#
A toolpath in Fusion is a neutral description of tool motion. A machine controller, however, wants a specific dialect of G-code, with its own header, tool change sequence, canned cycles, coolant codes, arc formats, and safety lines. The program that translates the neutral toolpath into the controller's dialect is a post processor, or simply a post.
Fusion posts are post configuration files with the extension .cps. A selection of generic post processors comes installed with Fusion and a wider choice can be downloaded from the online Post Library; you can edit a post, ask the Autodesk Community, or contact a provider on the Services Marketplace for customisations. Autodesk advises taking all necessary safety precautions when testing the NC file from any new post.
The post stage is where a correct simulation can still crash a machine. A wrong post can output the wrong units, the wrong work offset, a tool change without a retract, or arcs in the wrong plane. Treat posting as a step that deserves review, not a button press.
Where to find it#
- Milling > Actions > Post Process (opens the NC Program dialog with the active setup).
- Milling > Setup > NC Program (Fusion's NC Program reference lists it under the Setup panel; Create NC Program is also on the Setup panel) to create a grouped program from several setups.
- Manage > Post Library to browse, copy, import and export posts.
- Right-click an NC program in the Browser and choose Setup Sheet for a setup sheet.
The NC Program dialog#
Posting uses the NC Program dialog. Its Settings tab contains (the items shown depend on the machine and post):
| Field | What it does |
|---|---|
| Use machine configuration | Uses the post defined in the setup's machine |
| Post | The post processor to use; Choose from Library opens the Post Library |
| Use cascading post | Runs a secondary post after the first to produce an extra file (e.g. for verification packages) |
| Name/number | Program identifier made available to the post |
| File name | Output file name; defaults to Name/number; can use expressions |
| Comment | Header comment |
| Output folder | Where the NC file is written |
| Post to Fusion Hub | Uploads a copy to the Fusion web client |
| NC extension | File extension, usually set by the post |
| Unit | Inches, millimeters, or the document settings |
| Open NC file in editor | Opens the result after posting |
| Create in Browser | Adds an NC program to the Browser |
| Post Properties | Properties specific to the chosen post |
The Operations tab lets you deselect setups or operations, and has Reorder to Minimize Tool Changes, which groups operations that use the same tool. Click Post to write the file.
The post library#
The Post Library (Manage > Post Library) is divided into libraries:
- Fusion Library: generic posts from the online Post Library; updated whenever Fusion updates.
- Local: personal posts on your device. Customised posts should live here; posts stored with the installed posts are overwritten when Fusion is updated.
- Cloud: posts in the Data Panel under Libraries > Assets > CAMPosts, shareable across a hub. Cloud libraries require Enable Cloud Libraries in Preferences > General > Manufacture.
- Linked: a folder elsewhere on your device that you link to (right-click Linked > Linked Folder).
Use the Filters on the right (Capabilities, Vendor) to narrow the list, then drag a post to your Local or Cloud folder or use Copy and Paste. The toolbar offers Edit, Copy, Paste, Import and Export. To check for updated posts, machines and print settings each time Fusion restarts, select Automatically Get Latest Posts, Machines and Print Settings under Preferences > General > Manufacture > Optional Features. If your machine maker supplies a post, prefer it (general guidance).
Post properties#
Most posts expose configurable properties that change output without editing code; they appear in the Post Properties group of the NC Program dialog and are specific to the chosen post. The list below gives the kinds of options posts commonly offer (general guidance; your post may differ):
| Property type | Examples |
|---|---|
| Output formatting | Sequence numbers, separating words with spaces, showing notes |
| Safety | Safe start block, safe retract style |
| Tool handling | Preload tool, tool change type, optional stop |
| Coolant | M-code mapping |
| Cycles | Canned cycles on or off, rigid tapping, drill retract mode |
| Arcs | Helical moves, arc output format |
| Multi-axis | TCP, tilted work plane |
| Work offsets | Extended offsets, multiple fixture offsets |
If a post has operation properties, Fusion shows a dialog summarising which properties are added to which operations, and they appear on the operations' Post Process tab. Properties set here apply to that run and can be stored with an NC program.
Tip: Save a copy of a post you have tuned for your machine to your Local or Cloud library, with a clear name, so that property defaults stay with it.
Setup-level post settings#
Each Setup's Post Process tab includes Program Name/Number, Program Comment, WCS Offset, Multiple WCS Offsets (with Number of Instances and WCS Offset Increment) and Operation Order. The WCS Offset is mapped by the post to a zero-table index: 1 is normally the first available index (for example G54 on a Fanuc post). Confirm in the posted file; how offsets above 6 are written (for example G54.1 Pn) depends on the post.
Tool numbers and offsets come from the tool definitions (Post processor tab of the tool).
NC Programs#
The NC Program tool does three things: posts your operations to NC code, groups multiple setups for output as a single NC program with multiple fixtures and offsets, and creates documentation (setup sheets and tool lists). Use an NC program to combine setups on the same fixture or machine into one file, and to apply post settings once for a set. In the Browser, NC programs appear under NC Programs; with Create in Browser selected, posting adds one. Posting a single instance of a pattern is also possible.
Step by step: post a program#
- Ensure all operations are generated and simulation is clean.
- Make a setup active (or select an NC program) in the Browser.
- Click Milling > Actions > Post Process. The NC Program dialog opens.
- In the Post list choose a post, or choose Choose from Library and select one.
- Enter a File name and select the Output folder.
- Review Post Properties: safe start, units, line numbers, coolant mapping, tapping mode.
- On the Operations tab deselect anything to exclude; optionally tick Reorder to Minimize Tool Changes.
- Click Post. Warnings may appear for unsupported features.
- Open the output file and review it using the checklist below.
- Create a setup sheet for the operator.
Reviewing G-code: a checklist#
Never run a new program without reading its first and last lines and scanning the rest. At minimum:
- Header: program number, units (G20 or G21), plane (G17), absolute mode (G90), cancel cycles and compensation (G80, G40).
- Work offset: G54 (or expected one) before the first move.
- Tool call: T number matches the library, and the tool change is preceded by a retract to a safe position (G28 / G53) as the machine requires.
- Spindle: S value and direction (M3/M4) before cutting; value within the machine range.
- Coolant: M8/M7/M9 as intended.
- First rapid: moves to X Y at a safe Z before descending.
- Feedrates: F values plausible and in correct units.
- Canned cycles: G81/G83/G84 etc. with appropriate R-plane and depth; canceled with G80.
- Arcs: G2/G3 with I/J (or R) values consistent with the plane.
- End: spindle off (M5), coolant off (M9), retract, return to a safe position, M30.
Compare against a known-good program from the same machine when possible.
Setup sheets#
Right-click an NC program in the Browser and choose Setup Sheet (or use the Setup Sheets command), name it and choose a hub project folder, then Save. Autodesk lists the contents as: an image of the model from the current view, WCS information, size and orientation of the raw stock and finished part, number of tools, maximum Z travel, cutting and rapid distances, estimated cycle time, and detailed information for each operation. The Summary, Tool, Setup and Operations sections can be shown in different Configuration styles. It opens in your internet browser and can be printed with Ctrl+P. Excel setup sheets are also available. Printing one for the operator is a good habit.
Editing and customizing posts#
Posts can be edited: use Edit selected in the Post Library, or edit the .cps in an external editor. Autodesk points to the Autodesk Community forums, the manual on the online Post Library, and Services Marketplace providers for help. Typical edits (general guidance) are the start or end block, custom M-codes, line number format, coolant mapping and tool change handling.
Cautions: always keep an original, test with a dry run, and store customised posts in your Local or Cloud library, because the installed posts are updated (and overwritten) when Fusion is updated.
Options reference#
| Option | What it does | Notes |
|---|---|---|
| Post | Chooses the post | Must match the controller |
| Use machine configuration | Takes the post from the setup's machine | |
| Output folder / File name | Destination and name | Name/number by default |
| Unit | Output units | Verify on the controller |
| Open NC file in editor | Opens after posting | For review |
| Create in Browser | Adds an NC program | |
| Reorder to Minimize Tool Changes | Groups operations by tool | Operations tab |
| WCS Offset | Zero-table index | Setup Post Process tab |
| Multiple WCS Offsets | Repeats the setup at incremented offsets | Setup Post Process tab |
| Post Properties | Post-specific options | Safe start, canned cycles, tapping, etc. |
Tips and pitfalls#
Tip: Dry run first. Run the program with the Z offset raised well above the part (for instance +50 mm on the work offset), spindle off or low, and feed override reduced, watching the path in the air. Then lower the offset in steps.
Tip: Keep one post per machine, with notes in the file header about changes you made.
Warning: The post is not a safety system. Unit and offset errors in G-code can send the tool through the part, the vise, or the machine.
Note: see the manufacturing extensions page for what the Personal-use licence limits; the post processing topics checked here do not describe such limits.
Warning: A generic post may not know your machine's quirks (tool changer macro, coolant M-codes, rotary braking). Test every feature.
Practice exercise#
Post the drilling practice part from the drilling page twice: once with canned cycles enabled and once with them disabled (expanded). Compare the files.
Expected result (if your post supports canned cycles): the canned version has compact G81, G83 and G84 blocks followed by G80, while the expanded version lists each hole as explicit rapid and feed moves and is many times longer. Both should show the same coordinates and the same tapping feed.
Related#
- Setups and stock (program name and work offset)
- WCS and orientation
- Toolpath simulation
- Drilling, tapping and hole operations