| ID: | 4264 |
| From: | Stan Gammons <sg...@gmail.com> |
| Date: | Mon, 20 Jul 2020 22:32:44 -0500 |
| Subject: | Re: [pcb-rnd] new: 4 more netlist file formats |
| in-reply-to: | 4263 from ge...@igor2.repo.hu |
Hi Igor2!
I thought that was asking too much :)
Yes, I have the schematic on paper. I'll try what you described
below. Thanks for your help!
Stan
On 7/20/20 10:25 PM, gedau@igor2.repo.hu wrote:
>
> 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
> now.
>
> 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
> nest
>
> 7. place (move) your subcircuits then draw your tracks!
>
>
> B. pcb-rnd-only way, no schematics; you keep the schematics on paper/jpeg
> forever
>
> 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.
>
> HTH,
>
> Igor2
>
>
>
Reply subtree:
4264 Re: [pcb-rnd] new: 4 more netlist file formats from Stan Gammons <sg...@gmail.com>