A few questions: does the update pcb also take care of the netlist or do I need to do both?
Also, if I change a footprint it doesn’t replace the footprint where it is in the layout.I have to delete the existing footprint and place it all over again.
Also, if I change the 3d association file I seem to have to repeat the operation manually for each footprint in the layout. This is true even if I change the parameter in the footprint editor and do a save.
If I check the box to delete extra footprints it removes a bunch of plated holes that I put in that were in fact used, in the sense that they were connected to a net.
BTW I always hit the save button when changing footprints.
When you enter (at PCB) into footprint edition you can Update footprint from library (I am writing from memory) and in that function you can mark to update all footprints from library. I do it many times.
External netlist file and updating the PCB directly are two different, independent functions. The external netlist file is only for communicating the netlist to 3rd party software.
The “Update Footprint” function takes care of that if you have edited and saved the library footprint. Changes made directly to a board footprint aren’t propagated to other similar footprints (on purpose, of course).
“Netlist” can be interpreted here in two different ways. eelik revered to the external netlist file.
Eeschema / Tools / Update PCB from schematic … however, puts the “netlist” (As in a list of connections between pins) directly from Eeschema into Pcbnew.
This, and your use of the 3D association file suggests you are trying to use the wrong workflow.
With a normal workflow the schematic is the reference, and after you’ve drawn the schematic, you assign footprints to the schematic symbols, and this is what creates the association between schematic symbols and PCB footprints.
If you’ve done that, then Eeschema / Tools / Update PCB from schematic … (Or [F8]) puts both the whole netlist and all footprints into Pcbnew.
You can not create the association between schematic symbols and PCB footprints with the footprint association file.
Normally the association between schematic symbols and footprints is done via unique number (“Timestamp” in KiCad V5.1 and UUID in KiCad-nightly V5.99), and this is done implicitly when you create footprint links in the schematic symbols.
If it is a simple schematic, it’s easiest to simply empty the PCB, then do the footprint assignment in the schematic and do the Eeschema / Tools / Update PCB from schematic … (Or [F8]) once more. Pay careful attention to any lines with red text. Those are important errors. For example in the screenshot below, a new footprint (U2, a SOIC IC) is added to the PCB, but C3 can not be added to the PCB because it has no footprint assigned yet. You should fix that in the schematic untill you have no errors anymore in this step.
If this is new to you, you should spend some quality time with beginner tutorials for KiCad.
If you’ve got a PCB with a lot of manually imported and placed footprints, then it can be repaired, but not just with the footprint association file, because that does not create the association, it just changes it.
I don’t want to go too deep here. If you’re still having troubles, then zip the project and post it here and I can give you some steps to repair it in your particular case.
Thanks to all who replied. I am functioning OK in this in the sense that I can get work done, but certain things have seemed odd to me. Superficially it looks like I ought to be able to open a pcb file in a text editor and just fix stuff that the interface makes difficult for me to do (possibly because I don’t use it right), however in practice I find that often backfires. I think the primary reason has to do with the timestamps (5.1.10). I did just see that one of my errors was just not clicking the checkbox so that updating the footprints in the schematic fixes them in the layout. In my mind that would be the default,so I was not looking for that.
As for the 3d associations, I was saving after editing that parameter in the footprint file.
Parenthetically, I periodically suffer from kicad startup problems on windows 7 that have been documented elsewhere without a solution as far as I can tell.
Love the program though! I wish I had time to contribute to the development but I’m barely keeping up as it is.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.