Electronics Overview

Overview#

The Electronics workspace is Fusion's built-in ECAD environment. It grew out of EAGLE and keeps EAGLE's command line, ULPs and scripts; Autodesk's help describes it as a cloud-based platform. If you know EAGLE, most concepts transfer directly: a schematic describes connectivity, a board (PCB) describes physical copper, and a library supplies the parts for both. Fusion adds cloud-based data management, a 3D PCB document, and exchange with mechanical designs.

A typical project flows like this:

1. Create or choose libraries (symbols, footprints, components).
2. Capture the schematic: place parts, wire nets, assign values.
3. Run ERC (electrical rules check).
4. Switch to the board, define the outline, place components.
5. Set design rules, route, pour copper.
6. Run DRC (design rules check).
7. Generate manufacturing data with the CAM tools (Gerber, drill, ODB++, IPC-D-356 netlist, pick-and-place) and export the BOM.
8. Optionally switch the board to a 3D PCB and fit it into an enclosure.

Where to find it#

• In Home click New (or File > New), choose Electronics Design in the What do you want to design? dialog and click Create New. In the Common tab choose New Schematic or Reference a Schematic, and New PCB or Reference a PCB document, then Save.
• The Electronics Design document is the umbrella document that keeps the schematic, 2D PCB and 3D PCB documents synchronized. By default they open as separate tabs of one Fusion window; you can undock them side by side.
• A library opens as its own Electronics Library document, with a Content Manager panel listing Components, Symbols, Footprints and 3D Packages.

Step by step#

1. Start a new electronics design from the New Design menu and name it. It is saved in your Fusion project like any other document.
2. Open the schematic tab. On the Schematic toolbar choose Place > Place Components to open the Place Components panel, then double-click a component to open the Add dialog.
3. Drop a few parts, then draw nets with Net on the Schematic Design toolbar.
4. On the Design toolbar choose Switch > 2D PCB. If no 2D PCB exists, Fusion creates and links one. All components appear beside an empty default rectangular board, joined by airwires (thin lines for unrouted connections).
5. Save often. Schematic and 2D PCB stay in sync through Forward&Back Annotation, but only while both documents are open; if you edit one while the other is closed they go out of sync.
6. Use the Manufacturing toolbar (CAM Preview, CAM Processor, CAM Export, PickAndPlace, Export ODB++, IPC-D-356 Netlist) when ready to produce files (see the manufacturing page).

The command line#

Electronics retains EAGLE's text command line near the bottom of the window. You can type commands such as ADD, MOVE, ROUTE, NAME, VALUE, DRC, ERC, RATSNEST, RIPUP, GRID. The input is not case sensitive and keywords may be abbreviated when unambiguous. Command strings can be separated by semicolons, and the ASSIGN command (or the Electronics keyboard shortcuts tool on the Design tab) binds command sequences to function keys and key combinations. Scripts (SCRIPT, .scr files) and ULPs (RUN, User Language Programs) are supported and can automate repetitive work.

Tip: If a toolbar button is not where a tutorial shows it, type the command name in the command line. Command names have been far more stable than menu layouts.

Options reference#

Tips and pitfalls#

Tip: Treat the schematic as the source of truth for connectivity. Do not try to edit nets on the board directly; fix the schematic and the board follows.

Warning: Keep both the schematic and 2D PCB open while editing. Forward&Back Annotation only works while both are open, and edits made with one closed leave the documents out of sync.

Warning: Many online EAGLE tutorials use .sch / .brd files and the standalone EAGLE UI. Fusion can import EAGLE libraries (via the Library Manager) and KiCad files, but the UI, file storage and some limits differ.

Practice exercise#

Create a new electronics design. In the schematic, place a resistor and an LED, wire them with a net, then switch to the board. Confirm that both parts appear with an airwire between them, then return to the schematic and change the resistor value; check that the value is reflected in the board.

Anatomy of an electronics design document#

An electronics design in Fusion is a container with three kinds of content, and knowing which one you are editing explains most early confusion.

• Schematic and board. These are two views of one data set. The schematic holds sheets, parts, nets and values; the board holds the same parts with positions, layers, traces and polygons. Because the connection is live, an edit in one view appears in the other without any export step.
• 3D PCB. A separate document generated from the 2D PCB with Switch > 3D PCB (this replaced the old "Push to 3D PCB" workflow). It is covered on the 3D PCB page.
• Libraries. Parts come from library documents; use Update design from library to bring a design up to date with library changes.

Saving creates a version in the Fusion project history. If a board edit goes wrong, you can open an earlier version from the data panel instead of undoing dozens of steps.

Worked example: scoping a first board#

Suppose you want a 5 V to 3.3 V sensor node with an ESP32 module, one I2C sensor, a USB-C power connector and two LEDs. Before opening Fusion, write the budget:

Having these numbers up front tells you whether the project fits the free tier (see the limits page) and what to ask of the library: every one of those 22 parts needs a symbol, a footprint and ideally a 3D package, and the USB-C receptacle and ESP32 module are the two most likely to be missing or wrong.

Preferences worth setting before the first part#

Tip: Check the behavior of grid snapping before drawing a single net: if pins you place are off-grid, nets will appear to touch without connecting, and ERC will flag unconnected pins that look wired.

Command line recipes#

The command line is more than a legacy feature; it is the shortest route to bulk edits. Commands below follow the EAGLE grammar that Fusion Electronics retains. Run them one at a time at first and watch the status line.

A script file is just those commands one per line, saved with an .scr extension and run with SCRIPT filename. A script that sets the grid, hides all layers except routing layers, and loads your fabricator's rules is a useful ten-line starting file. If a command is rejected, the status line states why; the usual cause is that the command is only valid in the schematic or only in the board.

Failure modes during the first project#

Choosing between electronics and plain 3D modeling#

Use the electronics document whenever copper, schematic connectivity, or manufacturing output matters. Use plain solid modeling for a dummy board (a 40 x 25 x 1.6 mm slab with connector bodies) when you only need the enclosure and nobody will fabricate the board from your model. A dummy takes minutes to build and avoids libraries entirely. Switch to a real electronics document when the board outline must be exact, when you want connector positions to follow routing changes, or when the board will be ordered.

Practice exercise#

Extend the LED exercise into a measured mini-project.

1. Create an electronics design called led-tester. Place a two-pin header, a 330 ohm resistor and a red LED; connect with nets and label +5V and GND.
2. Compute the LED current: with a 5 V supply, a 2.0 V forward drop and 330 ohms, I = (5 - 2.0) / 330 = 9.1 mA. Put the value in a text note.
3. Switch to the board, move all parts onto a 25 x 15 mm rectangle drawn on the Dimension layer, and route them.
4. Use the command line to run DISPLAY NONE; DISPLAY 1 16 20 and confirm only copper and outline remain visible, then DISPLAY ALL.
5. Go back to the schematic, change the resistor to 680 ohm, and check the board value text. Recompute the current (4.4 mA).
6. Save, close, reopen, and confirm the project history contains at least two versions.

Related#

• Schematic Capture
• Board Layout
• Electronics Limits in Personal Use