Please see the attached image. “Error C2 pad 1 not found” is one of many similar reported DRC errors on a new PCB derived from a schematic. If I delete C2 from the schematic and replace it with the same exact part, the error disappears. Any idea what could be going on? I have 50 errors of this type reported by the DRC. I tested several parts - delete and replace then no error reported for that part. This seems a Kicad error but I may be making some nutty error in my layout. Thanks Al (San Francisco area)
PS- there is a similar warning for the same part that reports an error – Warning: no net found for component C2 pad N (and P).
Pad 1 and 2 are typical pad symbols.
Interesting is to find where from capacitor could have pad N and P (looks like someone name it as Negative and Positive).
In KiCad pad “numbers” can have both digits and letters. This makes it possible to use “chessboard” pin numbering in parts like BGA’s. But whatever combination you use, the pin numbers in the schematic have to match with the pin numbers in the footprints.
As far as I know it’s not recommeded to use the “basic” parts from the simulation library at all. Symbols from the regular device library work just as well, and I think the simulation directory is mostly still kept to maintain compatibility with old / legacy projects.
Okay, all great ideas! Yes I was copying my Spice schematic into my “board schematic”. BIG MISTAKE, Thanks for pointing this out. Plus I see that the symbol N/P, 1,2 dont align with the footprint due to using the Spice library symbols. Thanks to paulvdh, and retiredfeline for these great hints. I have some work to do to fix this…
So for future work, should I create two separate schematics, one for Spice sim and one for the “board”. This seems very inefficient and I suspect this is a common problem… Or, is there best practice I am missing? Cheers, Al
Yes, that’s the situation for the foreseeable future. Your simulation schematic will be somewhat different anyway; it will have signal sources, probes, etc.
True the Spice diagram is somewhat different due to sources and other Spice specific “parts”. But, as least for my case, 90% of the Spice version is the same as the board version. Thanks again for the advice. As with most problems one aspect of the solution is “never assume…”. Al
It is possible to use the same schematic both for simulation and for creating the PCB. Spice sources and such can be excluded from the PCB, while connectors can be excluded from the Simulation, or maybe even add a model to simulate parasitic cable properties to it. Another important point is that Spice models often use different pin numbers. If you want to use the schematic for both, then the pin numbering in the symbol has to match the actual footprint, while you can use a pin number translation table for mapping the pin numbers to the spice model.
Another important detail is that (symbols for) spice models sometimes have the anode and cathode swapped compared to real-life footprints, so be sure to triple check that. (But in real life there is no standard for diode orientation either, so you’d have to check that anyway.)
Changing a whole lot of symbols in bulk is also easy in KiCad. Just use Schematic Editor / Tools / Edit Symbol Library Links.
For the rest, you also have to think about whether it makes the most sense to use a single schematic for both the PCB and ngSpice. If the circuits are nearly the same, then it makes sense, but often you just want to simulate small sections. Then it’s probably more convenient to make a few small projects for the simulation, and when it works, use copy and paste to get those sections into the main project.
There are also many more ideas then KiCad developers, and they have a backlog of several years, but it is the intent to make it easier to use schematics both for simulation and creating the PCB. A recent addition to KiCad-nightly was to add an option to exclude a whole schematic sheet (in a hierarchical design) from the simulation.
In my case device schematic has nothing common with Spice schematic.
I use Spice only to check supply π filters characteristics using for all elements sub-circuits with their parasitic components.
I use separate KiCad configuration when working with Spice (having only Spice libraries) and separate for PCB design (having no spice libraries in library list).
