Fusion 360 Electronics documentation from EAGLE (direction, multiple pins/parts/sheets, @, invoke, ...)
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
This is an explanation of some of the mysterious features in Fusion 360 Electronics, the documentation of which hasn't made the jump from EAGLE's help PDF (and often wasn't brilliant there, either...).
Background: CadSoft's EAGLE "Easily Applicable Graphical Layout Editor" was aquired by Autodesk in 2016 and subsequently repackaged as the rolling-beta that is 'Fusion 360 Electronics', so I mostly refer to these instructions as applying to EAGLE (hoping that Fusion 360 Electronics will reintroduce these features/processes in a more logical manner).
The English & German manuals in PDF from EAGLE 9.6.2 are attached.
(Pin) Direction
When creating the Symbol layer of a Component in an Electronics Library, the purpose of a pin is defined via its "direction". The EAGLE help file defines direction on p. 273:
The Direction parameter specifies the logical direction of the signal flow:
NC Not connected
In Input
Out Output
IO Input / output
OC Open-collector / open-drain
Hiz High-impedance output
Pas Passive (resistors, etc.)
Pwr Power pin (power supply input)
Sup Power supply output for ground and supply symbols
The benefit of setting the appropriate direction is to Rule Checks, allowing EAGLE to check for obvious errors.
Also, both 'power' directions result in automatic connection to supply nets, which can simplify matters (e.g. GND to GND) but also cause issues (e.g. in design with multiple "VCC" or a supply connector with an unused voltage rail). [You might think that 'Pwr' (power supply input) pins must be connected, while 'Sup' (power supply output) pins may be connected, but no, it is 'must' in both cases.]
Pins with the Same Name / @ Symbol
Based on p. 303.
If one symbol/footprint has multiple pins with the same name, e.g. several GND pins, use the 'at' / @ symbol in the name, e.g. GND@0, GND@1, GND@2, ... (zero- and one-based indexing both work).
The official glossary definition of the @ symbol remains a mystery.
Layers and their Usage
Based on p. 349.
Most layer names are self-explanatory, some non-obvious ones:
In 2D PCB and Footprint Editor
20 Dimension Board outlines
39 tKeepout Restricted areas for components, top side (ditto for 40 bKeepout)
41 tRestrict Restricted areas for copper (trace) (esp. autorouter), top side (ditto for 42 bRestrict)
The differences between 47 Measures, 48 Document, 49 Reference and 51 tDocu are still a mystery to me.
In Schematic, Symbol and Components Editor
97 Info Additional information/hints
98 Guide Guidelines for symbol alignment
Placing hidden Parts / Invoke
Based on pp. 140, 141.
EAGLE / Fusion 360 Electronics is designed to use multiple symbols ("Parts") within one Component; e.g. for a hex inverters IC, placing the Component might simply give one Part: one inverter symbol with only input & output pins. The IC's power pins are not shown, but are probably automatically connected to the VCC and GND nets (using the 'Pwr' pin direction). How then do you put a bypass capacitor on the VCC pin? Invoke. How do you put one of the inverters on a different sheet? CTRL + RIGHT CLICK.
Components with several Parts
The placing of parts from within a component depends on their "Add Level". If it is set to "add=next", repeat left-clicking will place the additional parts. Some parts are set to "add=request" and can only be placed via the Invoke tool. (I cannot find documentation on the options of Add level = { "must", "can", "next", "request", "always" }.)
The Invoke tool can be accessed by selecting Invoke from the right-clicking menu of a symbol or from the ribbon bar (MODIFY), or you can type /invoke. Then select the Part you wish to place (limited to one Part per Invoke).
Placing Parts from one Component across multiple Sheets
For example, you might have an IC containing multiple logic gates, and might want to put one of the gate Parts on a different Sheet to the rest of the Component.
Option one: using Invoke via command line.
1. Take note of the name of the Component, e.g. U201, where you have already used it.
2. Change to your target Sheet.
3. Press [/] or LEFT-CLICK into the command line
3. Enter e.g. invoke U201
4. Select the Part you want from the GUI.
Option two: using Move via the mouse (and keyboard).
0. Make sure the Sheets pane (with thumbnails) is visible.
1. Invoke and place the additional Part symbols you want on the Sheet where the Component was first placed.
2. Select the Part symbols you want to move (forms a 'Group', necessary even if only one Part).
3. Select the Move tool.
4. [CTRL] + RIGHT-CLICK one Part from the Group (binds the Group to the mouse cursor)
5. LEFT-CLICK into the target Sheet
6. LEFT-CLICK to place the Group.
Dollar sign / $
EAGLE uses the dollar symbol / $ in names, e.g. pins might be P$1, P$2, P$3, ... There seems to be no issue with removing the $ symbol and no benefit to keeping it. I suspect the $ sign tells EAGLE it is a auto-increment serial number (if there is aready a G$1, the next G$1 placed it will make G$2, but if it was G1, EAGLE would not make the next G1 into G2), but cannot find any documentation on it.
