ID: | 4263 |
From: | ge...@igor2.repo.hu |
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 <sg...@gmail.com> |
replies: | 4264 from Stan Gammons <sg...@gmail.com> |
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:
4263 Re: [pcb-rnd] new: 4 more netlist file formats from ge...@igor2.repo.hu
4264 Re: [pcb-rnd] new: 4 more netlist file formats from Stan Gammons <sg...@gmail.com>