Additive Settings and Machine and Material Libraries#
Overview#
Besides handing a mesh to an external slicer, Fusion's Manufacture workspace can describe and output an additive job itself. According to Autodesk's help, an additive setup is built from two library items:
- Machine - chosen from the Machine Library, which holds definitions for CNC machines and additive printers. The machine fixes the additive technology (FFF, SLA/DLP, MJF, SLS, MPBF, eBeam, binder jetting or DED), and later options narrow to that technology.
- Print setting - chosen from the Print Setting Library. A print setting is a collection of parameters associated with an additive machine and is specific to the bulk raw material (for example ABS or PVA). For FFF, common parameters include layer height, extrusion width and infill pattern. Any post processor is set in the print settings.
The help describes no separate additive "material library": the raw material is represented by the print setting. Setups do not need a work coordinate system or stock; Autodesk recommends setting +Z to Up on the ViewCube.
Which technologies are supported, and which steps need the Fusion Manufacturing Extension, depends on the machine. Autodesk marks MPBF, eBeam and DED workflows, additive process simulation and several support types (such as Volume and the Polyline family) as extension features.
Where to find it#
- Manufacture workspace > Additive > Setup > New Setup opens the Setup dialog. Machine > Select opens the Machine Library and Print Settings > Select opens the Print Setting Library.
- Machine Library folders: Fusion Library (read-only definitions from Autodesk), My Machines with Local, Linked (external folders) and Cloud subfolders, Document (machines used in the current design) and Recent. To edit a Fusion Library machine, copy it into My Machines. Selecting a machine copies it into the Document folder, where it can also be edited.
- Print Setting Library folders: Fusion Library (generic print settings) plus Cloud and Local folders. Copy a close match into Cloud or Local to edit it.
- Cloud libraries must be enabled in Preferences > General > Manufacture > Enable Cloud Libraries.
Step by step#
Creating an additive setup#
- Open a model, then in the Manufacture workspace choose Additive > Setup > New Setup.
- Next to Machine, click Select. In the Machine Library, filter by Technologies to shorten the list. If your printer is missing, use the generic Autodesk machine for the technology (for FFF the help uses the Autodesk Generic FFF Machine in the Fusion Library) or build your own definition.
- If the machine has no print settings, or you want different ones, click Select next to Print Settings and choose one (the FFF tutorial uses the Fusion Library setting ABS 1.75mm).
- Leave Operation Type on Additive; it is set from the machine type.
- Click OK. For the FFF workflow in the help, clicking OK generates an additive toolpath, and the Browser shows a setup node with a machine node whose Platform, Build Volume and Additive No Build Zone can be toggled.
- Position, arrange and support the parts as described in the sibling pages.
- Simulate with Actions > Simulate Additive Toolpath, then Post Process to create the NC program (G-code) for FFF. For other technologies use the Create Machine Build File tool.
Print settings: select, edit, presets#
- Edit a print setting in the Print Setting editor. General parameters apply to all bodies on the platform; body presets can differ per body. You can create a preset and assign it to a body.
- Copy and paste print settings between libraries, import and export them, and delete them from the Print Setting Library. For MPBF or eBeam machines Autodesk documents a way to overwrite print settings.
- Parameters describing how supports are built are in the Print Setting editor.
- Name your copies clearly (general guidance), for example with material and layer height.
Custom machines#
Autodesk documents a workflow for using and creating machine definitions and a Machine Builder; the machine definition includes a Platform page where a .3mf can define a Platform No Build Zone. Machines can have a linked post processor. The exact fields of the additive machine editor are not covered in this guide; see the Machine Library reference in Autodesk's help. Start by copying the closest machine and test with a short print before trusting a large job (general guidance).
Output files#
The Create Machine Build File tool saves a build to a type compatible with your machine, and the available types depend on the machine in the setup. Autodesk-generic types include G-Code (.gcode), CLI ASCII and Binary (.cli), LSR (.lsr), SLC (.slc), SVG ZIP, PNG and TIFF; vendor-specific types (for example Formlabs .form, Prusa SL1/SL1S, EOS, Renishaw, Trumpf) appear only in a matching vendor machine setup. This tool is for MPBF, eBeam, SLA/DLP and SLS machines. The 3MF Scene Export tool writes a 3MF that, unlike STL, retains details such as supports, and works for FFF, MJF, SLA/DLP, SLS, MPBF, eBeam and binder jetting machines. Note from the help: vendor formats can shift loose elements or generated supports, so avoid stacking elements on top of one another before exporting. Sending an MJF build to HP SmartStream needs the HP 3D Printers for Autodesk Fusion add-in from the Design and Make Marketplace.
Sharing libraries#
Use the Cloud folders for team sharing (after enabling Cloud Libraries), Linked machine folders to manage definitions centrally, and the import/export options to share print settings by file. Keep a naming convention (general guidance).
Options reference#
| Item | What it holds | Notes |
|---|---|---|
| Machine | Additive or CNC machine definition, technology, build volume/platform, optional linked post processor | Fusion Library is read-only; copy to My Machines to edit |
| Print setting | Parameters for the raw material and process (FFF: layer height, extrusion width, infill pattern); post processor | General parameters plus per-body presets |
| Body preset | Per-body overrides of print settings | Create, then assign to a body |
| Library locations | Fusion Library, Cloud, Local (print settings); plus Linked, Document, Recent (machines) | Cloud needs Enable Cloud Libraries |
| Setup | Machine + print settings + models | Models: Autodesk recommends components rather than bodies |
| Create Machine Build File | Machine-specific or generic print file | MPBF, eBeam, SLA/DLP, SLS |
| 3MF Scene Export | 3MF including supports | FFF, MJF, SLA/DLP, SLS, MPBF, eBeam, binder jetting |
| Process simulation | Thermo-mechanical analysis of MPBF builds, predicts displacement and recoater interference | Fusion Manufacturing Extension; MPBF machines only |
Tips and pitfalls#
Tip: Copy and rename; do not rely on editing the read-only Fusion Library entries. Autodesk states that Fusion Library machines must be copied into My Machines to edit.
Tip: General guidance: library values are starting points. Calibrate on your own printer and save the tested settings as your own print setting.
Warning: General guidance: a wrong start G-code block or post processor can crash the nozzle or set wrong temperatures. Compare the first output with known-good slicer G-code and watch the first print.
Warning: Check units: the FFF workflow in the help begins by setting the document units (Inch or Millimeter) through the Units entry in the Browser.
Tip: If no native toolpath is available for your printer, use the setup for positioning and supports where offered and export a 3MF to your slicer, or skip the setup and use Export or Print Utility from Utilities > Make > 3D Print.
When to use the Fusion setup instead of an external slicer#
This comparison is general guidance, not Autodesk data.
| Use the Fusion setup when | Use an external slicer when |
|---|---|
| You want orientation, supports and plates tied to the parametric model | Your printer vendor provides tuned slicer profiles |
| You are preparing metal builds and have the extension | You need slicer-specific FDM features such as variable layer height or modifiers |
| You manage a team library of machines and print settings | You just want the quickest path to print |
| You want additive and subtractive in one environment | Your slicer better supports your firmware |
Practice exercise#
Create an additive setup for a part of your choice with the Autodesk Generic FFF Machine and the ABS 1.75mm print setting from the Fusion Library. Arrange the part, add a Solid Volume Support if it has overhangs, simulate the toolpath and open the print statistics (Autodesk documents a Display Print Statistics tool for FFF, MPBF and eBeam). Then copy the print setting into your Local folder, rename it, change the layer height, regenerate and compare the statistics. Expected result: a different layer height changes print time noticeably. As general guidance, compare the estimates with your slicer's; large gaps usually come from differing wall, infill or speed settings.
Related#
- Orientation and Support Generation
- Build Plate Arrangement and Nesting
- SLS and Metal Additive Basics
- Licenses and plans (01-getting-started)
- Preferences (01-getting-started)
Maintaining libraries over time#
A library is only useful if it stays trustworthy. Treat it like a small piece of engineering documentation and apply a few habits.
Version your profiles. When you change a print setting, do not silently overwrite the old one. Save a new entry such as PETG_0.2_standard_v2 and note in the description what changed and why (for example, "lowered nozzle temperature 5 C to reduce stringing"). If a later print regresses, you can return to the previous profile in seconds.
Tie profiles to a physical spool or batch. Filament brands differ, and even the same brand varies between colors. For dimensionally critical work, create a material entry per brand and color you actually use, and record the measured filament diameter. A 1.75 mm filament that actually measures 1.72 mm shifts extrusion by several percent.
Record the printer state. Nozzle diameter, nozzle material (brass, hardened steel), build surface and firmware version all influence results. Put them in the machine's description field so that the profile is not misused after a hardware change. If you swap to a 0.6 mm nozzle, create a new machine entry rather than editing the old one.
Audit shared libraries. In a team, designate one person to approve changes to cloud libraries. Periodically delete unused entries, and keep a short entry describing the naming convention.
Back up. Export local libraries to files and store them with your project archive. If you reinstall Fusion or move computers, restoring a library is far easier than reconstructing dozens of tuned values from memory.
Check after updates. After a major Fusion update, open a recent setup and confirm the machine and print setting still resolve and that the print statistics still match your last build (general guidance).