Libraries, Symbols, Footprints and Devices

Overview#

A part in Electronics is not one object but a chain of linked objects:

• Symbol - the schematic drawing with pins.
• Footprint (called package in EAGLE-era documentation) - copper pads, silkscreen and mask for the board.
• 3D package - an optional 3D model attached to the footprint for 3D PCB.
• Component - the glue (called a device in EAGLE). It lists one or more symbols (gates), assigns a footprint (package variant), and maps each symbol pin to a pad.

Understanding this chain lets you fix wrong pinouts, add parts that do not exist, and keep libraries tidy.

Where to find it#

• In the schematic, Place > Place Components opens the Place Components panel, which lists components from your active libraries.
• The Electronics Library Manager (Library tab > Libraries > Open Library Manager, or the Open Library Manager icon in the Place panel) sorts libraries into Hub (shared with your team), Public (provided by Autodesk or third parties, read-only) and Private (Library.io or local disk). Activating a library only changes your own Place panel.
• To create a library use File > New Electronics Library. The library editor has a Content Manager panel on the left for Components, Symbols, Footprints and 3D Packages; double-click an asset to open its editor.
• Designs hold their own copy of library parts. Use Update design from library (pick one or more libraries) or Update design from all libraries used in design to refresh them.

Step by step#

Create a new part#

1. Create a new library or open one you own.
2. Symbol: click New Symbol, name it, and draw on layer 94 (Symbols) with the Draw tools. Set the grid to 0.1 inch or 2.54 mm, then use Pin (or PIN). In the Pin dialog set Function (None, Dot, Clk, DotClk), Length (Point, Short, Middle, Long), Display (Direction, or Direction and Pin name), Direction (nc, in, out, io, oc, pwr, pas, hiz, sup) and SwapLevel; right-click rotates the pin. Place >NAME on layer 25 (NamesTop) and >VALUE on layer 27 (ValuesTop) with the TEXT command.
3. Footprint: click New Footprint (or import an existing one, optionally with its connected 3D package). Use Place > PTH Pad or Place > SMD Pad (or the array variants) and set sizes from the datasheet's land pattern. Draw the silkscreen on layer 21 (SilkscreenTop), documentation graphics on layer 51 (DocumentTop), and add >NAME and >VALUE texts. Mounting holes use the Hole (NPTH) command.
4. 3D Package (optional): click New Package, then use the Package Generator (pick a sample package such as SOIC, adjust the specification tabs, click Update), model it with Solid tools, create it from an existing design, or upload a local STEP file. A component with no 3D model is replaced by a placeholder rectangle in the 3D PCB.
5. Component: click New Component (Create group). Use Add to bring in the symbol (gates are named G$1, G$2 and so on, with Addlevel and SwapLevel fields), add a package/footprint via the Content Manager (New package, or New > Add local package > Import), then Connect each pin to its pad(s).
6. Save and place the new device in a schematic to test.

Edit an existing part safely#

1. Public libraries are read-only; use Fork public libraries (Library Manager) or import the component into your own library.
2. Fix the issue (for example a pin number mismatch), then use Update design from library.

Options reference#

Tips and pitfalls#

Warning: The most common cause of a dead board is a pin-to-pad mapping error in a home-made device. Print the footprint 1:1 and compare with the physical part before ordering.

Tip: Draw the footprint's pad-1 marker clearly on the silkscreen layer. Autodesk's footprint instructions list no courtyard layer; they name layer 51 (DocumentTop) for documentation graphics and layers 39/40 (ComponentExclude) and 41/43 (RestrictCopper, RestrictVias) for keep-out areas.

Tip: Use Autodesk's library search and community libraries for common parts, but inspect each. Copy from a reliable source into your own library and keep that library under version control.

Warning: Libraries are copied into designs. Fixing a library does not retroactively fix old boards; run the library update command or replace the part.

Tip: Import EAGLE libraries through Library Manager > Hub Libraries > Sync libraries > Import EAGLE Libraries (it reads libraries.rc), or upload a local .lbr through the Data Panel. Autodesk recommends importing the private packages too, to avoid permission errors when teammates build 3D boards.

Practice exercise#

Create a library my-parts. Build a 3-pin voltage regulator in a SOT-223 footprint: symbol with IN, GND, OUT; footprint from the datasheet land pattern; device mapping pins to pads. Place it in a schematic, switch to the 2D PCB, and compare the pad positions with the datasheet drawing.

Worked example: building a SOT-23-5 regulator footprint from a datasheet#

Datasheets give a recommended land pattern or the package dimensions. Suppose the datasheet gives a SOT-23-5 body 2.9 x 1.6 mm, five leads on a 0.95 mm pitch (three on one side, two on the other) and a recommended pad of 0.6 x 1.1 mm with 2.6 mm between pad centres across the body.

1. Set the footprint grid to 0.05 mm. Pad coordinates are then easy to enter.
2. Place SMD pads 1, 2, 3 (Place > SMD Pad) at x = -0.95, 0, +0.95 and y = -1.3, and pads 4 and 5 at x = +0.95 and -0.95, y = +1.3. Each is 0.6 wide by 1.1 tall, roundness 0.
3. Draw the silkscreen body at 2.9 x 1.6 mm, then move it so the lines sit 0.2 mm outside the pad edges where they would otherwise touch the pads (silkscreen on pads is cut by the fab and shows up as DRC warnings).
4. Add a pin-1 dot on the silkscreen outside the pad, and, if you want a keep-out, a rectangle 0.25 mm beyond the pads and body on a ComponentExclude layer.
5. Check by printing at 1:1 on paper and laying the physical part on it: all five leads must land on their pads with at least 0.2 mm overlap beyond the lead tip.

Clearance across pad rows is the usual error: mistaking the datasheet's overall lead span (2.8 mm) for the pad-centre distance (2.6 mm) pushes the pads outward and weakens the solder fillets.

Pin-to-pad mapping and gate rules#

A swap level of 0 prevents exchanging gates at all; a level of 1 allows exchange with other gates at the same level. Use 0 for the power gate and 1 for identical logic gates; power gates are usually given Addlevel Request.

Naming conventions that pay off#

• Footprint names that include the true size, for example R0603, C0402, SOT23-5, QFN-32-5X5-EP3.7. Avoid "RESISTOR" as a name because two different tolerances and sizes are not distinguishable.
• Component names including the manufacturer part number root, such as TPS7A3301.
• A library per project family: passives, connectors, ics-power, custom-modules. A single huge library makes search slow and makes version control diffs unreadable.
• Prefix: R, C, L, D, Q, U, J, SW, TP for test points. The BOM and silkscreen follow it.

Making a 3D package fit#

If you generate a 3D package from standard dimensions, check three values: body length and width, body height above the board (including standoff), and pin 1 orientation. A generic QFN body with a 0.85 mm height and 0.02 mm standoff sits flush; a through-hole electrolytic capacitor needs its body height, typically 11 mm for a 100 uF 16 V radial part, set explicitly for enclosure fit. Position the model's origin at the footprint origin so rotations behave. If the model appears rotated, fix the model rather than rotating the footprint, because rotating the footprint changes pad coordinates relative to the datasheet (general guidance; Autodesk's help does not describe a specific rotate control).

Library management workflow#

1. Keep Autodesk and vendor libraries read-only and copy devices into project libraries.
2. When a part is re-used, check the 3D package, mask and paste layers before first use, and record the check as a note on the device description.
3. After editing a library part used in open designs, use the library update tools in each design. Update one design first and inspect the result before updating all.
4. For distributor-provided symbols and footprints, put them through a checklist: pin count, pin names, pad size, pad pitch, drill sizes, orientation of pin 1, 3D model alignment.
5. Version your libraries: save a dated copy before bulk edits; if the Fusion project supports versions, use the version note field.

Checklist before trusting a custom part#

Failure modes and fixes#

Practice exercise#

Build the SOT-23-5 regulator above as a complete part and prove it.

1. Create library power-ics. Draw a symbol with pins IN (1), GND (2), EN (3), NC (4), OUT (5), directions in, pwr, in, nc, out respectively; choose directions that match the datasheet.
2. Create the footprint with the pad coordinates above. Print it at 1:1 and check against a physical part or a datasheet drawing printed at the same scale.
3. Create the component and map pins to pads 1 to 5. Add the manufacturer part number as an attribute.
4. Generate a 3D package (Package Generator) at 2.9 x 1.6 x 1.1 mm and verify it sits on the pads in the 3D view.
5. Place the part in a schematic with a 1 uF capacitor on input and output, switch to the 2D PCB, and measure the pad centre distance across the body with the measure tool; it should be 2.6 mm.

Related#

• Schematic Capture
• 3D PCB and ECAD-MCAD Sync
• Board Layout