kicad/doxygen/eagle-plugin-notes.txt

Eagle Plugin Implementation Notes.  2017 Russell Oliver

Below is some notes on the correspondence between Eagle schematics and symbols libraries and the
KiCad equivalent.

Eagle libraries are a many to many listing of symbols and footprints connected by a device set and
device definitions. They are embedded in the schematic and board files if there are used, and
therefore the schematic symbols and footprints can be recovered from either file.

An Eagle device set definition is the information needed to represent a physical part at the
schematic level including the functional gates of the device. Each gate is lists the symbol to be
displayed for that gate. This is equivalent to a KiCad symbol unit. Since the symbol is defined
outside of the device set, multiple devices sets in the library can use the same symbol for a gate.
Lower to a device set, is the device definition. This establishes the link between the schematic
symbols and a physical part through the 'connect' elements. These map the symbol pins for each gate
to the physical pins provided by the package (footprint) definition. An Eagle Symbol outlines the
layout of graphical of items including pins.  Pins for multi gate symbols are generally labelled
per their function, i.e. input / output. An Eagle symbol pin is not numbered but merely labelled. A
connect element gives the pad number for each pin found in that gate.  Therefore the equivalent
KiCad pin number is read from the connect element pad number. Since an Eagle gate is equivalent to
a KiCad symbol unit, the graphical items for that unit will be copied from the Eagle symbol for
that gate and will be unique for that unit. This will yield duplication of the graphical elements
if the same symbol is used for multiple gates but the conversion will be complete.

An Eagle sheet contains a list of instances, which are equivalent to KiCad schematic component
entries. An instance describes the part, the gate used and its location on the sheet. This is
translated into the equivalent KiCad symbol with the given unit number.

Eagle 'plain' items describe graphical items with no electrical connection, such as note text,
lines etc. Of importance is the use of wire elements to describe both electrical connections and
graphical items. A wire element will act as an electrical connection when defined within a net and
segment. Anywhere else it is a graphical line. The layer for the wire element will change the
displayed colour for the wire. Connections between regular wires and busses occur when a wire ends
on a bus segment. When translated to KiCad a bus connection symbol is created. Within an Eagle
schematic there can be multiple sheets in a flat hierarchy. For each sheet, there is a list of
electrically connected nets. Each net is broken up into graphically connected segments, defined by
a list of wires and labels. Labels remain associate with wires of that net segment, even if they
are not located on a wire element. This necessitates the movement of such a label to the nearest
wire segment within KiCad.