Overview#
Bringing a file into Fusion looks simple: pick a file, wait, get a model. Behind that simplicity there are two distinct mechanisms and one important background process. Knowing them explains most of the behavior people find confusing, such as why an uploaded file appears in the Data Panel before you ever open it, why a SolidWorks assembly takes minutes to appear, and why a file you opened is not the same object as the file on your disk.
The mechanisms are:
- Upload sends a file from your computer to the cloud project you have chosen. Fusion then translates it server-side into a Fusion design (for CAD formats) or stores it as-is (for other file types).
- Open from my computer is a convenience that performs an upload and then opens the resulting design in a single step.
- Autodesk Translation is the service that converts foreign formats into Fusion's native representation. It runs in the cloud, which is why you need an internet connection to import most vendor formats, and why large imports can sit in a queue.
A second family of commands, Insert, brings data into an already open design (a mesh, an SVG, a DXF, a decal). It is covered in the import options page.
Where to find it#
| Action | Location | Notes |
|---|---|---|
| Upload | File > Upload in Fusion; Upload button in the web client | Drag files in or Select Files; Change Location picks the project |
| Drag and drop | Drag files into the Drag and Drop Here area, or into a project in the web client | Equivalent to Upload |
| Open from my computer | File > Open > Open from my computer | Opens directly, or shows Job Status for designs that need cloud translation; click Open in the Action column when done |
| Open from the Data Panel | Double-click a design | Opens the cloud document |
| Job status | Data Panel, Job Status (a clock/list icon, or the Job Status dialog) | Shows queued, running and failed translations |
| Insert | Insert menu (Insert DXF, Insert SVG, insert designs); Insert Mesh on the Mesh tab | Inserts into the current document |
Menu labels vary slightly between releases; verify in your version.
Step by step#
Uploading a file#
- Open the Data Panel (the grid icon at top left).
- Navigate to the project and folder where the file should live. Uploading into the wrong project is the most common mistake; the destination is a real, shared location, not a scratch area.
- Click File > Upload. In the dialog, drag files into the Drag and Drop Here area or click Select Files. (In the web client, Upload offers File or Folder, and From Dropbox; folders cannot be uploaded from Dropbox.)
- Review the list. For assemblies made of many files, choose the whole folder so Fusion can resolve the references between parts.
- Click Upload. A job is created; the file appears in the panel when the upload completes, and its thumbnail may take longer than the file itself.
- Watch Job Status if the translation is large. When the status reads complete, double-click the new design to open it.
Opening directly#
- Choose File > Open > Open from my computer.
- Select the file. Fusion uploads it to the project that is currently active in the Data Panel, then opens it.
- If the file is an assembly with referenced parts located in the same folder, make sure all parts are in that folder before you start, otherwise the references may come in broken.
Uploading an assembly from another CAD system#
- Gather the assembly file and every referenced part file into one folder, preserving the folder structure the original CAD system expects. SolidWorks assemblies expect to find parts relative to their saved paths; Inventor uses project files.
- In Upload, select the folder, or select all files and let Fusion detect the top-level file.
- When prompted, confirm which file is the top-level assembly. Fusion will translate the parts and create a design for the assembly that references them.
- After translation, open the assembly and check the browser for broken (red or missing) references and check that component origins landed where you expect.
Options reference#
| Option / control | What it does | Notes / default |
|---|---|---|
| Upload destination | Project and folder that will own the translated design | Defaults to the folder currently selected in the Data Panel |
| Select Files / Change Location | Chooses files and a different destination if needed | In the web client, uploading a folder opens the Upload Assembly dialog with an auto-detected parent file you can override |
| Job Status | Lists translation jobs with success, running or failure states | Failed jobs normally include a short reason; keep a screenshot for support |
| Open from my computer | Upload plus open in one step | Creates a persistent cloud document; it is not a temporary view |
| File references of non-Fusion designs | Not preserved when uploading with Fusion | Autodesk says to use Desktop Connector on Windows to keep references |
| Supported types | See the format cheat sheet | Depends on license; blank Personal Use cells in Autodesk's table mean a commercial subscription |
| Store non-CAD files | Some other file types (PDF, images, spreadsheets, STL) may be stored in the project without conversion | Stored files can be viewed or downloaded but not edited as designs |
How Autodesk translation actually behaves#
The translation service reads the foreign file's geometry and, where it can, structure such as assemblies, names, colors and units. What it cannot do is reconstruct the original feature history. The result is a "dumb" solid: a body or set of bodies whose faces are exact, but with no sketches, extrudes or parameters behind them. In the timeline you will typically see a single base feature or none at all, depending on the import path and your design history setting.
Some consequences follow:
- Geometry is exact for BRep sources. A SolidWorks part or a STEP file carries real curved surfaces, so holes stay round and fillets stay fillets. You can measure them, offset them, and use Press Pull or Direct-style edits on them.
- Structure is partially preserved. Assemblies usually arrive as components with names and positions. Mates and constraints from other CAD systems are generally not converted into Fusion joints; rely on the positions and re-create joints if you need motion.
- Appearances are approximate. Colors usually transfer; named materials with physical properties often do not. You may need to reapply Fusion appearances.
- Metadata varies. Part numbers, descriptions and custom properties may or may not survive. Check the Properties of the translated component.
- Large files queue. Translation is a shared cloud resource; a hundred-megabyte assembly may take several minutes. This is normal.
Tip: If a file was exported from another system as both its native format and a STEP file, try both. Native translation sometimes preserves more structure; STEP is sometimes cleaner because the sender's own software wrote it. Keep whichever opens better.
Tips and pitfalls#
Tip: Upload into a dedicated "Imports" folder in the project. It keeps third-party data separate from your own designs, and it makes it obvious which files are pristine originals.
Tip: Rename the translated design immediately. Fusion usually names it after the file, including the version suffix you may not want to propagate into your own part numbers.
Warning: Open from my computer does not link the cloud document to the file on disk. If the sender sends a revised file, uploading it again may create a new version only if you choose the existing design to update; otherwise you will get a second, unrelated document. Use the Data Panel's upload-as-new-version function (look for it in the context menu of the existing design; verify in your version) to preserve history.
Warning: Translation failures are usually one of: a corrupt file, a file from a newer CAD release than the translator supports, missing referenced files, or an assembly too large for the service. Try the same part from the sender's software as STEP before concluding the file is bad.
Warning: Do not upload confidential third-party data to a shared hub project without checking your sharing and NDA obligations. Anything uploaded lives in Autodesk's cloud and is visible to project members.
Tip: If Job Status shows a long-running job, you can keep working. Fusion notifies you when the document is ready. Closing the application does not usually cancel a job already accepted by the cloud, though you should verify in your version.
Working offline#
Because most translations run in Autodesk's cloud, a fully offline session cannot import vendor formats. Fusion has an offline mode, but its capabilities for importing translated files are limited. If you know you will work on a plane, translate the files ahead of time and let them sync to the local cache; the cloud documents then open offline. Native F3D files and STEP files are the most reliable to open, but "most reliable" is not the same as "guaranteed"; plan accordingly.
Practice exercise#
- Download a freely available STEP file of a small assembly (for example, a fastener set or a gearbox from a public library).
- Create an "Imports" folder in a scratch project.
- Upload the file using the Data Panel, then watch Job Status until it completes.
- Open the design and expand the browser. Count the components and confirm they have sensible names.
- Measure the diameter of one hole and one outer cylinder with the Inspect > Measure tool. Compare with the values documented by the source.
- Try Open from my computer for the same file and notice that it creates (or offers to create) another document. Delete the duplicate.
Expected result: you can explain the difference between Upload and Open, you have seen translation status, and you know what the imported model does and does not contain.
Related#
- Import options: units and orientation (import-options-units-orientation)
- Data loss and large files (data-loss-and-large-files)
- Data Panel basics (01-getting-started/data-panel-basics)
- Hubs and projects (01-getting-started/hubs-and-projects)