Fusion 360 import guide

CircuitHub imports Autodesk Fusion (formerly Fusion 360) electronics designs from the CAM Processor ZIP that Fusion exports. It holds the two sets of files CircuitHub needs:

• The manufacturing files: Gerber X2 layers, drill files and a Gerber job file. These give us the copper, solder mask, paste, silkscreen, board outline and drill layers.
• The ODB++ export, a zip inside the CAM ZIP. This gives us the bill of materials, footprints and part placements.

Gerber files on their own cannot be imported, and Fusion's own design files (.fbrd, .fsch, .f3z) are not recognized. If you prefer, you can export the board and schematic in the legacy EAGLE format instead of the ODB++ data; see Using the EAGLE format instead.

Before you upload

Save your design, then export from that saved version.

Export the CAM Processor ZIP

1. Open your board in Fusion. On the Manufacturing tab, choose CAM Processor.

   

2. In the CAM Processor dialog, check that:

   • Export as ZIP is selected.
   • Units is set to Metric.
   • In the Gerber section, Output type is set to Gerber X2.
   • In the Gerber section, Include job file in gerber export is selected.
   • The ODB++ output is left in place. Fusion's default CAM job writes it, as CAMOutputs/ODBFiles/<job>.zip inside the ZIP, with the EDA data (parts, footprints and attributes) included.

   

3. Choose Process Job and save the ZIP file.

Fusion's default CAM job also writes the drill file, drill_1_16.xln, into the ZIP. Keep it: CircuitHub needs at least one drill file that goes through the whole board.

Uploading

Upload the CAM Processor ZIP. The upload page unpacks it for you and keeps the ODB++ zip inside it whole, as one file: it shows as ODB++ · <job name>, and the Gerber, drill and job files show with their layer functions. Do not unpack the ODB++ zip yourself; if you upload its contents as separate files they are not recognized.

The assembly text files and the odb_job.odbjob file from the ZIP are not recognized. They do no harm; ignore or remove them to keep the list tidy.

The upload page marks drill_1_16.xln as plated holes through all layers and asks you to confirm this. Check that this matches your drill file: if it does, choose Confirm; if not, open the row's … menu and choose Edit drill details to change it.

If your board has blind or buried vias, Fusion also writes a drill file for each layer pair, such as drill_1_2.xln. Choose Set drill details on each one and give its layer span, counting copper layers from 1 at the top down to the bottom layer. These numbers can differ from those in the file name, where Fusion always numbers the bottom layer 16: on a four-layer board that uses Fusion layers 1, 2, 15 and 16, drill_2_15.xln spans layers 2 to 3. After the import, check the number of blind/buried layer sets in the board options on your project page.

Once every drill file is confirmed, the upload page shows Ready to import as an ODB++ project from your gerbers.

Required files

• One ODB++ zip, the CAMOutputs/ODBFiles/<job>.zip from the CAM Processor ZIP, kept whole.
• The Gerber files for every copper layer and exactly one board outline (profile.gbr), together with the solder mask, paste and silkscreen layers that Fusion exports.
• At least one drill file that goes through the whole board (drill_1_16.xln from the default CAM job).

Without the Gerber files

If you upload only the ODB++ zip, the upload page asks whether to make the board from the layers in the ODB++ data; choose Use the ODB++ layers to continue. Fusion's own Gerber files match your design best, so upload the whole CAM Processor ZIP when you can.

Recommended

• The Gerber job file, gerber_job.gbrjob. CircuitHub reads your board thickness from it and checks that it lists the same number of copper layers as your Gerber files. Only one job file is allowed.

Optional BOM

You can also upload a BOM in either .csv or .tsv that conforms to the supported format.

Where your data comes from

Add manufacturer part numbers as attributes on your parts, such as MPN or ManufacturerPartNumber; see Specifying part numbers in EDA tools. Parts without pads, such as logos and fiducials, are not in the ODB++ export and are left out.

Fusion does not always write VALUE into the ODB++ data. Parts with the same footprint and no value, description or part number share one BOM line; give those parts a part number attribute, or supply a CSV BOM.

CircuitHub does not read do-not-place (DNP) settings or assembly variants from Fusion designs; every placed part imports as fitted. Mark DNP parts on CircuitHub after the import, or use the DNP column of a CSV BOM.

Using the EAGLE format instead

Instead of the ODB++ data, you can supply the board and schematic exported in the legacy EAGLE format together with the same manufacturing files. The schematic adds the symbols CircuitHub uses to check polarity. Upload one or the other: an ODB++ zip and EAGLE files in the same upload count as two design tools, and the import is blocked until you remove or ignore one of them.

Make the two exports from the same saved version as the CAM Processor run. CircuitHub cannot tell when the board and schematic files come from different versions, so whenever you change the design, make the board and schematic exports and the CAM Processor run again.

Export the board file

1. With the board open, open the File menu and choose Export….

   

2. Set Type to EAGLE 9.X Compatible Board Files (*.brd) and choose Export.

   

Export the schematic file

1. Switch to your schematic, open the File menu and choose Export….

   

2. Set Type to EAGLE 9.X Compatible Schematic Files (*.sch) and choose Export.

   

Uploading EAGLE files

Upload the .brd file, the .sch file and the CAM Processor ZIP together, then ignore or remove the ODB++ zip the page unpacks from it. The board and schematic show as Board · Eagle and Schematic · Eagle, the drill files are confirmed as above, and the page shows Ready to import as an Eagle project.

With EAGLE files, the data comes from:

• Parts, footprints and placements: the board file.
• Values and descriptions: both files, matched by reference designator. Where they differ, the schematic wins.
• Manufacturer / distributor part numbers: the schematic's part attributes, and the attributes set on the device or technology in its library.
• Symbols, used to check polarity: the schematic.

Parts that are in the schematic but not on the board are left out.

The EAGLE 9.X compatible export is an XML file. Binary .brd and .sch files from EAGLE 5 and earlier are not supported; the upload page asks you to re-export them as XML.

Single design

Only upload files from a single design at a time. Supplying files from different designs leads to ambiguities during import.