40 lines
3.0 KiB
Plaintext
40 lines
3.0 KiB
Plaintext
|
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.
|