ID:	701
From:	ge...@igor2.repo.hu
Date:	Tue, 30 May 2017 08:21:50 +0200 (CEST)
Subject:	[pcb-rnd] up next: subcircuits (a.k.a. footprint model redesign)
replies:	702 from miloh <fr...@gmail.com> , 707 from John Griessen <jo...@cibolo.com>
Hi all,
 
now that pcb-rnd 1.2.3 is out, it's time to celebr^W focus on the next big 
chunk of work.
 
A few months back we made a feature poll among pcb-rnd users about which 
feature was the most wanted. The result was:
 
1st: editable layers (just released)
 
2nd: subcricuits (see below)
 
3rd: pad stacks and blind/buried vias (with the lowest score possible - seems 
to be a lower priority task with no real user demand, postponed for a later 
date)
 
So next big chunk is subcircuits: footprint model redesign.
 
Current situation: pcb elements
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
 
There are a lot of feature requests out there about extending the footprint 
model. A few random example:
 
- polygon in footprint, 2009, 2010 
http://archives.seul.org/geda/user/Sep-2010/msg00619.html
http://archives.seul.org/geda/user/Jun-2009/msg00370.html
 
- arc in footprint, 2010:
http://archives.seul.org/geda/user/Apr-2010/msg00613.html
 
- how to work around missing mask editing feature in footprints, 2004:
https://www.mail-archive.com/search?l=geda-user@seul.org&q=subject:%22Re%3A+gEDA-user%3A+PCB%3A+how+to+clear+soldermask+from+entire+footprint%22&o=newest&f=1
 
It would be possible to add code just for these cases. However, each such 
example would introduce a new set of special cases in the code base, and these 
cases will always interact with almost all other such specil cases. Which means 
an exponential growth in special case vs. sepcial case interaction that would 
be rather hard to maintain long term. This is not the route we take in pcb-rnd.
 
Generally speaking, the problem is that our footprint model is a bag of special 
cases: footprints can have the special objects, for example:
 
  - element-line, but that's only lines drawn on silk
 
  - (smd) pad, which can't have arbitrary shape and must be on top or bottom 
copper
 
  - pin, which is basically just an "element-via", with some pin number and pin 
name attached; mostly code dup of via plus code dup from smd pads for the 
number/name
 
  - exactly 3 silk text objects, from which only 1 can be dispalyed at any given 
time (refdes, footprint description, value)
 
  - a bunch of automatic side effects, like mask and paste on smd pads
 
There are some clever hacks to work around some of the limitations, usually by 
combining pads and pins. But this is not building from pure, orthogonal bricks, 
but building from fuzzy haystacks, mainly trying to combine and cancel side 
effects. I know this "works", I know we do this since forever, but this is far 
from the optimal solution.
 
 
Future: subcircuits
~~~~~~~~~~~~~~~~~~~
I am going to slowly replace this old mechanism in pcb-rnd with a new system 
called "subcircuits". From the user's point of view, a subcircuit takes the 
same role as a "footprint" (... in a lib, or "element", when placed on a board 
- as of gEDA/pcb terminology).
 
A subcircuit does not have special objects like "pins", "pads" or 
"element-lines". Instead, it has the same objects that the layout has: lines, 
arcs, polygons, text and vias. (In fact I am going to use the same C struct 
that the board uses, which is pcb_data_t in pcb-rnd).
 
Trick #1: flexible layer handling
 
Just like a board, a subcircuit also has a layer stack. When the subcircuit is 
a footprint, this layer stack is not a particular physical stack, rather a 
recipe. E.g. instead of fixed layer numbers, this stack would contain patterns 
like "this layer should be in the top copper physical layer on the board". It 
could indirectly reference any physical layer: copper, silk, mask, paste, 
outline; top, bottom or even inner layers. Once the subcircuit is placed on a 
board with an actual physicla layer stack, the layer binding is performed: with 
or without interactive user intervention, using the layer stack recipe, each 
layer the subcircuit uses is boud to one of the actual layers of the board.
 
Trick #2: flexible terminal handling
 
Just like in tEDAx, pins/pads are no special objects but plain drawing 
primitives tagged for a given terminal. Terminal is the "pin number, pin name" 
concept. A multiple vias, lines, arcs, polygons or even text objects can be 
tagged to be part of a terminal. The netlist sees terminals only.
 
Result:
 
In practice this means our new footprints will be capable of hosting:
 
- arbitrary shaped pads drawn as lines and polygons
 
- arbitrary shaped copper objects not being pads; a.k.a. pcb antenne; but this 
includes copper text or mask cutout text too; your company logo can really be a 
footprint
 
- arbitrary mask cutouts, mask cutouts that are not derived from pads
 
- arbitrary placement of paste; want a grid of paste blobbs on the center pad 
of your largish qfn? no need t emulate it with 10 pads, just draw them on the 
paste layer
 
- slots or other cutouts/edge-contour-patterns; even the whole board shape can 
be a footprint
 
- text and polygon on silk
 
 
Schedule
~~~~~~~~
 
This will probably take a long time, spanning multiple development cyclces, 
just like the layer rewrite did.
 
Stage 1:
 
We will start implementing it in the current cycle and will make it gradually 
grow until it reaches its full featured, final form. We will make sure that at 
every intermediate release subcircuits are usable and alreayd provide extra 
features over footprints. We will keep the original footprints in place during 
this process.
 
Lihata board v3 will have support for subcircuits. The subcircuit subtree will 
also be avaialble as a subcircuit file format for sharing footprints.
 
While we are in this stage, we'll encourage users to use subcricuits instead of 
footprints, and always save in lihata board v3 instead of other formats. 
However, the code will still be able to use the old footprints in parallel.
 
Stage 2:
 
At some point in time subcircuits will be capable enough to replace footprints. 
At this point we will remove footprints, pins, pads, element-lines, 
element-arcs. We will also need to rewrite import code to convert old elements 
to subcricuits on load and rewrite export code to convert subcircuits back to 
elements for old formats.
 
Stage 3:
 
We'll convert pcblib from the old, element based .fp files to lihata subcircuit 
files. We'll rewrite the parametric footprint scripts to generate lihata 
subcircuits instead of pcb elements. This will include extending some of the 
parametrics with features that was not possible with pcb elements because of 
the limitaiton of the model/format.
 
(This also means our parametric footprints won't be available for pcb mainline 
without a conversion or without mainline upgraded to lihata formats and the 
subcircuit model)
 
 
 
What you can do to help
~~~~~~~~~~~~~~~~~~~~~~~
 
Most wanted: testers. We are again going to change a critical part of the 
system, we need all sort of testing. Testers with even only a few hours a week 
are very valuable for getting such new features stable.
 
Second most wanted: contributors on non-coding material (e.g. docs, tutorials, 
test files)
 
Production users: people who use the stable version of pcb-rnd for actual 
production boards and report bugs. Especially those who are willing to try out 
new features that are already labelled stable by developers.
 
Programmers: we have a growing number of developers and contributors, but 
there's always more work than resources, obviously. Anyone is welcome if they 
have some free time and willing to accept the pcb-rnd ways of doing things. Be 
part of one of the most dynamic projects of gEDA!
 
Regards,
 
Igor2
Mailing list archives : pcb-rnd

Navigation
