Overview#
Fusion is a cloud-connected CAD/CAM/CAE/ECAD application, and almost every project eventually touches somebody else's software: a customer sends a STEP file, a laser shop wants a DXF, a printer slicer wants a 3MF, a colleague lives in SolidWorks. Understanding file formats is therefore not an optional extra. It is the difference between a clean hand-off and a day of repairing broken geometry.
The first thing to internalize is that file formats fall into a handful of families, and the family matters far more than the three-letter extension. Each family stores a different kind of information:
- Native (history-bearing) formats store the full design: sketches, features, parameters, the timeline, appearances and, for assemblies, joints. In Fusion that is F3D and F3Z. In Inventor it is IPT/IAM, in SolidWorks SLDPRT/SLDASM.
- BRep (boundary representation) exchange formats store exact geometry: faces defined by mathematical surfaces (planes, cylinders, NURBS) joined at edges, plus topology and often color and assembly structure. STEP, IGES, SAT and SMT belong here. They do not carry your feature history.
- Mesh formats store a surface approximated by thousands of flat triangles (or quads). STL, OBJ and 3MF belong here. They are ideal for printing and visualization but are not precise and cannot be edited as features.
- 2D formats store drawings, outlines or vector art: DXF, DWG, SVG, PDF.
- Vendor and application formats exist to move data between particular ecosystems: Inventor, SolidWorks, CATIA, Rhino, SketchUp, FBX, USD and so on.
This page is a map of those families. The companion pages go into the workflows: how to bring files in, how to send them out, and how to avoid the data loss that each family can cause.
Warning: The exact list of supported formats, and which of them can be exported rather than only imported, changes between Fusion releases and depends on your license tier. Autodesk's "Supported file formats" help page states that all listed formats are supported with commercial subscriptions and that a blank Personal Use cell means the format requires a commercial subscription. IGES export and DXF export through File > Export are commercial only; every license can export a sketch as DXF with Export DXF. See the format cheat sheet for the full table.
Where to find it#
There is no single menu for "formats". Instead, format choice appears in several places:
| Task | Where | Notes |
|---|---|---|
| Upload a file to the cloud | File > Upload (or Upload in the web client) | Drag files in or Select Files; Change Location picks the project |
| Open a file directly | File > Open > Open from my computer | Same family list as Upload |
| Insert into an existing design | Insert Mesh (Mesh tab > Create), Insert > Insert SVG, Insert > Insert DXF, plus Insert designs | Format-specific insert commands |
| Export a design | File > Export | Choose a Type: F3D/F3Z, 3MF, Inventor, DWG, DXF, FBX, IGES, LMV (.svf), OBJ, SAT, SketchUp, SMT, SPD, STEP, STL, USDZ |
| Export a sketch | Right-click a sketch in the browser, Export DXF | 2D only; unit selectable |
| Export a mesh body | Right-click a body or component in the browser, Save As Mesh | STL (binary or ASCII), OBJ, 3MF |
| Export a drawing | Drawing workspace, Output or the export-PDF/DWG commands | Covered in the drawings section |
Menu names move occasionally as Autodesk reorganizes the interface; treat the labels above as the common ones and verify in your version.
Step by step#
Use this procedure whenever you need to decide which format to use. It takes thirty seconds and prevents most interop problems.
- Identify the receiver. Who or what will consume the file: a person using other CAD, a slicer, a CAM post-processor, a renderer, a web viewer, a laser cutter?
- Identify what must survive. Do they need exact curved faces, a feature tree they can edit, colors, units, assembly structure, or only a visible shape?
- Pick the family. If they need to edit features, the only real answer is the same CAD system's native format, or rebuilding. If they need exact geometry, choose a BRep exchange format. If they need a printable shape, choose a mesh. If they need outlines, choose a 2D format.
- Pick the specific format inside the family. For BRep, STEP is the default. For mesh, 3MF is the modern default and STL the universal one. For 2D, DXF for machines and PDF for people.
- Test the round trip. Re-import your own export into a new empty design and check dimensions, units and orientation before sending it anywhere.
Options reference#
Native Fusion formats#
| Format | Extension | What it carries | Notes |
|---|---|---|---|
| Fusion Archive | .f3d | A single design with its history, bodies, components, appearances | The portable "save a copy" format; no external references |
| Fusion Archive with references | .f3z | A design plus all the referenced external designs it depends on, zipped | Use for assemblies built from separate documents; verify extension behavior in your version |
| Fusion Design cloud document | (no file; stored in hub) | Same data as F3D, versioned in Autodesk's cloud | Primary working format in Fusion; see the Data Panel page |
An F3D is essentially a snapshot. When you export one from a document that has external references, the references may be pulled in or broken depending on how you export, which is why F3Z exists. Both can be re-imported into Fusion with full history, and nothing else can read them with history.
BRep exchange formats#
| Format | Extension | Typical use | Notes |
|---|---|---|---|
| STEP | .step, .stp | The neutral standard for solids and assemblies | Best default; read and written by essentially every CAD tool |
| IGES | .iges, .igs, .ige | Older surface-oriented exchange | Weak with solids and assemblies; export needs a commercial subscription |
| SAT | .sat, .sab | ACIS kernel exchange | Import and export (.sat); only ACIS up to version 7 can be uploaded |
| SMT | .smt | Autodesk's ShapeManager-flavored sibling to SAT | Common between Autodesk products (Inventor, AutoCAD, Fusion) |
| Parasolid | .x_t, .x_b | Kernel format used by SolidWorks, NX, Solid Edge | Import only (not in the Export list) |
Mesh formats#
| Format | Extension | Carries | Notes |
|---|---|---|---|
| STL | .stl | Triangles only, no units, no color | Universal for printing; binary or ASCII |
| OBJ | .obj (+ .mtl) | Triangles/quads, UV coordinates, materials | Common for rendering and game pipelines |
| 3MF | .3mf | Triangles plus units, color, materials, metadata | Modern successor to STL for printing |
| FBX, USD | .fbx, .usdz | Scene data, hierarchy, materials | FBX for exchange with 3ds Max, Maya and similar; USDZ for AR (ASCII English characters needed in path and file name; unsupported appearances become Steel Satin) |
2D formats#
| Format | Extension | Typical use |
|---|---|---|
| DXF | .dxf | Exchange of 2D geometry with laser, waterjet and other 2D CAM |
| DWG | .dwg | AutoCAD-native drawings; availability depends on license tier |
| SVG | .svg | Vector artwork imported as sketch geometry |
| Human-readable drawings; export from the drawing workspace |
Vendor and application formats#
Fusion's import list typically includes Inventor (IPT, IAM), SolidWorks (SLDPRT, SLDASM), CATIA V5, NX, Creo (Pro/E), Solid Edge, Rhino (3DM), SketchUp, Alias (WIRE), JT, Autodesk Eagle files and others. In the Export list only Inventor (.ipt, .iam) and SketchUp (.skp) appear among these; the others are import only. Consult the current supported-formats table for your plan. SolidWorks drawings (.slddrw) cannot be opened. Import of a vendor format is almost always a translation: Fusion reads the geometry and sometimes the assembly structure, but the original feature tree is discarded.
Tips and pitfalls#
Tip: When in doubt, ask the receiver which version of which format they want. "STEP" has several application protocols (AP203, AP214, AP242), and a customer's CAM package may only accept one. See the STEP best-practices page.
Tip: Keep a native F3D (or the cloud document) as your source of truth. Treat every exchange file as a disposable export, regenerated on demand, never as the master.
Warning: A file extension tells you the container, not the quality. A STEP file may contain exact solids, or it may contain a mesh converted to thousands of tiny planar faces. A DXF may contain true arcs or hundreds of line segments approximating them. Open the file and look.
Warning: Round-tripping through a lossy format repeatedly (Fusion to STL to Fusion to STL) compounds errors. Go back to the master design for each new export.
Warning: Personal-use licenses restrict some formats and export functions (for example IGES export and File > Export of DXF). If a format is missing from your Type list, check your license before assuming a bug.
Practice exercise#
- Create a new design and model a simple bracket with at least one hole, a fillet and a curved face.
- Save it as a cloud document, then use File > Export to write the same bracket as F3D, STEP and STL into a scratch folder.
- Compare the file sizes. Expect the STL to be a different size from the STEP, and note that the F3D is compressed.
- Open each file into a new design (Open from my computer). Confirm that only the F3D shows a timeline with features, the STEP shows a single body with no history, and the STL arrives as a mesh body that you cannot extrude-edit.
- Measure the same hole diameter in each. The STEP should match exactly; the STL will show a faceted approximation.
Expected result: you can describe, from experience, which family each file belongs to and what it preserved.
Related#
- Format cheat sheet (format-cheat-sheet)
- Mesh vs BRep exchange (mesh-vs-brep-exchange)
- Data Panel basics (01-getting-started/data-panel-basics)
- Mesh workspace and import (07-form-sculpt-mesh/mesh-workspace-and-import)