My 2c.
One of the fantastically useful features of eeschema is components have
an "arbitrary" list of key:value pairs (fields) attached to them as
attributes.
Can I suggest that such a feature attached to objects on the PCB would
be even more powerful/useful.
It would mean that changes like the ones suggested would not require
further format changes to the pcb file, these attributes can be
added/deleted at will as they are just a key:value pair. It would also
make the file format backward/forward compatible, pcbnew wont care what
the key:values are, it can read/edit/propagate them. If functionality
exists to utilise them then it can use it, if not, they are passive,
just like eeschema.
Further, the key:value pairs in eeschema could be imported into the
matching pcb objects, so that there is only 1 place that needs to be
edited to set them (the schematic). (I actually think that should be the
proper place to set them)
And by objects I mean both components AND nets. At the moment only
components have "fields" on the schematic, the ability to attach them to
nets would be mighty handy.
It would also be super useful for python scripting, because you can
tag/parametrise your objects on the pcb and your scripts can then,
easily, only do things with the appropriately tagged entities.
FOR EXAMPLE:
On the schematic, a key value pair is added to a net:
IMPEDANCE:50
This attribute is set as visible, so when the schematic is printed its
OBVIOUS that the net needs to be 50Ohm impedance. (It would be great on
schematic if the visible flag had 3 states: invisible, value only,
key+value)
On the PCB, a python script is run "adjust_impedance", it scans all nets
looking for ones with the "IMPEDANCE" key, and then adjusts the width of
the trace to have that impedance, as required. And if it can't, it
generates a list of nets which are not the correct impedance, based on
the board parameters as set in the schematic.
ALL of the features suggested below would be easier to implement with
such a unified attribute system between schematic/pcb AND would mean
that fewer changes need to be made to the file formats long term.
Steven J
On 03/05/16 20:40, Tomasz Wlostowski wrote:
Hi all,
Recently there has been a lot of discussion on these features. Here's a
short proposal how we could hit all three birds with one stone:
Changes to SCH:
- none
Changes to netlist import:
- auto_generate flag for SCH components - when set, invokes a Python
script/C++ plugin which updates the PCB footprint of the component
depending on its SCH parameters (e.g. produces a microstrip footprint
based on Width/Length parameters defined on SCH).
- write some microwave component generator plugins (or port the existing
tools). Perhaps a good job for Python.
Changes to PCB:
1) Add two flags to each graphical primitive within a footprint:
- net_tie: DRC treats the primitive as non-conducting and doesn't throw
a short circuit error (see drawing A)
- net_inherit = pad_number: the primitive will take the net of the pad
with given pad_number (see drawing B)
2) Add new 'anchor' virtual pad type.
- indicates the point to attach a trace/via when routing the component.
- exists on a single copper layer.
- has no physical copper.
- has an optional direction vector which denotes how it can be connected
with a trace/other anchor pad (see drawing C)
- has a circular perimeter (maybe other shapes in the future if needed).
Objects intersecting the graphical primitive outside the anchor
perimeter are considered colliding by the DRC (see drawing D) even if
they have the same net.
3) modify .kicad_pcb/footprint formats to support the above:
- extend fp_* entities: net_tie & net_inherit flags
- extend pad entity: add anchor pad type, perimeter radius and direction
vector.
4) modify DRC to support the above (we can benefit from the work already
done by JP)
Advantages:
- microwave footprints generated straight from the schematics.
- net ties for free (since based on the same idea as microwave components)
- custom footprint copper shapes almost for free (costs one extra flag &
some changes in netlist importer)
- minimum changes to file formats & data structures.
The attached drawing shows use cases for all of the above and explains
the concept of anchors.
Looking forward to your feedback,
Tom
_______________________________________________
Mailing list: https://launchpad.net/~kicad-developers
Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
Unsubscribe : https://launchpad.net/~kicad-developers
More help : https://help.launchpad.net/ListHelp
_______________________________________________
Mailing list: https://launchpad.net/~kicad-developers
Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
Unsubscribe : https://launchpad.net/~kicad-developers
More help : https://help.launchpad.net/ListHelp
