Mailing list archives : pcb-rnd

Date:Tue, 21 Jul 2020 05:25:07 +0200 (CEST)
Subject:Re: [pcb-rnd] new: 4 more netlist file formats
in-reply-to:4262 from Stan Gammons <>
replies: 4264 from Stan Gammons <>
On Mon, 20 Jul 2020, Stan Gammons wrote:
> I guess importing a jpeg of a schematic is asking too much?
That's asking for writing an AI. AI is out of the scope of pcb-rnd.
I can imagine someone writes a stand alone jpeg->schematics converter AI. 
It won't be me, tho. Anyway if it ever happens, whatever schematics 
editor they choose for output, we probably can already import from that so 
our side of the flow would be fine.
> What would be
> the best/easiest way to make a somewhat simple through hole board from a
> schematic?
There are mainly three methods for this. Because of yourprevious question 
I am going to assume you have your schematics on paper/jpeg.
A. the nice, clean, semi-automated/fulli-digitized way, which requires you 
to use a schematics editor software:
1. If your schematics in jpeg, first draw it in a schematics editor. Pick 
your favorite schematics editor, we really support a wide range of them by 
2. Make sure you specify the value and footprint for every component you 
have in the footprint. Some users will say you should name every net too 
(but that's optional). Make sure footprint names you used in the 
schematics are recognized by pcb-rnd (they are in your footprint library) 
- easiest way is using the library window of pcb-rnd and just type in 
footpritns in the filter entry to see if you already have that footprint 
in your lib. Don't forget parametric footprints, like dip(8), dip(14), 
dip(anyevennumber), acy(300), rcy(300). If you have a footprint that our 
minimal library we ship with pcb-rnd doesn't contain, check on edakrill.
3. Then export a the netlist from the schematics capture software you use 
in whatever format we import as netlist.
4. File menu, import, import schematics -> choose the file format from the 
combo box, click on import. If you did everything properly, you'll already 
see the footprints placed on your board.
5. you probably want to run the disperse subcircuits operation (it's in 
the Connect menu) or manually move apart the footprints heaped
6. press {c r} (that's a 'c' then an 'r' on the keyboard) to get the rats 
7. place (move) your subcircuits then draw your tracks!
B. pcb-rnd-only way, no schematics; you keep the schematics on paper/jpeg 
1. take your parts from the schematics one by one; open the librayr window 
with {w l}, pick a suitable footprint and place your subcircuit somewhere 
on the board
2. hover over the footprint and press {e r}; this lets you change the 
refdes; make sure you set it to whatever the schematics says. Save when 
you finish!
3. when all footprints placed and named, select the rats layer on the left 
and the line tool on the top; then take each net line from you schematics, 
check what component/pins are connected by that network and just draw 
those _logical_ connections. Whenever you are creating a new network, 
pcb-rnd will ask for the net name. Thus you are building a full blown 
netlist manually, without a schematics editor! When done, save.
4. At this point you effectively have "manually imported" a netlist, 
pcb-rnd is keeping track on it, so you can switch to method A's point 6 
and do the layout as usual.
C. digitize the netlist using your text editor (no sch editor needed)
1. Pick a suitable netlist format pcb-rnd supports; spice won't work, you 
need something that supports footprints (we support like 10 of such 
formats). I'd obviously use the tEDAx netlist format, that one is well 
documented and very easy to understand and write by hand.
2. Take your favorite text editor, create a new text file and start 
writing a netlist tracing things manually from the schematics; how exactly 
you do it depends on the format you pick. But generally you are going to 
write a list of parts (typically listing refdes, footprint, value for 
each) and a list of nets (typicall a netname and a list of 
refdes-pinnumber connections). When you are done, save the file.
3. From this point you can follow method A from point 4. importing your 
netlist and routing your board.

Reply subtree:
4263 Re: [pcb-rnd] new: 4 more netlist file formats from
  4264 Re: [pcb-rnd] new: 4 more netlist file formats from Stan Gammons <>