Footprint associations; update PCB from schematic

Software
1

The issue behind my earlier suspected bug:

seems that my schematic footprint assignments seemed to be getting over-written by the footprint assignments in my symbol library. When the symbol library did not specify a footprint (I did that for resistors and capacitors for example) that may have caused the disconnection.

Tools>Update PCB from schematic gives me this dialog box with the upper 3 tick boxes:
image

If the bottom tick box is unchecked, does that change the footprint assignments as listed in the schematic symbol properties?

Has there been ANY change in the default behavior of these three tick boxes for my version, particularly the bottom one related to footprint assignments?

As for the second question, there would seem to be a number of possibilities, including:

  1. No memory whatsoever between cycles of “Update PCB from Schematic”.
  2. Memory of the settings within a KiCad session.
  3. Memory for a project.
  4. Memory for an installation of a given KiCad version.
  5. I suspect there could be others.

I could probably spend a lot of time with experimentation in an effort to figure the above, but this may not give me all of the answers. I assume that someone knows??

Thanks.

Application: KiCad x64 on x64

Version: 8.0.6, release build

Libraries:
wxWidgets 3.2.6
FreeType 2.13.2
HarfBuzz 9.0.0
FontConfig 2.14.2
libcurl/8.8.0-DEV Schannel zlib/1.3.1

Platform: Windows 11 (build 22631), 64-bit edition, 64 bit, Little endian, wxMSW
OpenGL: Intel, Intel(R) Iris(R) Xe Graphics, 4.6.0 - Build 31.0.101.5186

Build Info:
Date: Oct 14 2024 01:02:33
wxWidgets: 3.2.6 (wchar_t,wx containers)
Boost: 1.85.0
OCC: 7.8.1
Curl: 8.8.0-DEV
ngspice: 43
Compiler: Visual C++ 1939 without C++ ABI

Build settings:

2

The whole thing is a big mess, I’m not even trying to understand it. I’ll comment only on the specific detail with a specific answer.

Yes, if the Update process is creating a connection between an existing footprint and a symbol, or keeping an existing connection, and the footprint library link (“library:footprint”) is different in the symbol Footprint field and in the PCB.

Whether you update using references or UUIDs, it’s possible that an already existing footprint in the PCB is linked to a symbol but the footprint, i.e. its library link, is different than in the symbol’s Footprint field. You may have changed the footprint in the PCB; then the old UUID is kept. Or you may have used reference designator for updating and that third checkbox unchecked; the UUID is created even if there’s mismatch between the library links.

That checkbox selects whether the footprints which have different library link than in the schematic symbols will be changed in the PCB so that the new footprints are chosen according to the schematic.

It should not affect any other footprints, namely those whose library links are already matched between the schematic and the PCB.

If you have used only the basic workflow, without the “Re-link” option, and so that after adding a footprint to the PCB you haven’t changed the symbol’s Footprint field, the third option should have no effect at all. It doesn’t update or change anything if there’s nothing to change. It doesn’t check, for example, if the symbols or footprints in libraries have been changed.

3

I don’t understand. You speak about possible “memory”. There’s no memory involved, only three or four things which I already mentioned:

  • Symbol’s Footprint field in the schematic, the footprint “library link” in form of “library:footprint”.
  • Reference designator.
  • UUID which is invisible for the user but exists in the schematic symbol and in the PCB footprint as the primary link between the symbol and the footprint in the design. (Not in the library symbol or library footprint; they don’t have UUIDs.)
  • Footprint’s library link in the PCB.

These are the only things which are “remembered” in this process.

4

Thank you very much. I appreciate your effort to dig into these details

With the three binary tick mark variables, there are 2^3=8 possible combinations for the state of those tick boxes. I did not knowingly check or uncheck any one of the three. The three boxes seemed to come up checked by default. Isn’t that one of 8 possible states of the 3 boxes remembered somehow? If it is not remembered then it would come up at random, which I doubt. If it always comes up (default) with all three checked, then at least that default state is remembered somehow in KiCad. But let’s say that I now uncheck the first box and save my project.

  1. Without closing the project, a few hours later I again update the pcb from schematic. Would that first box remain unchecked?

  2. What if I close the project and re-open it?

  3. What if I turn off my computer after closing the project, and then re-open the project?

  4. What if I close the project and open a different project?

  5. What if I update to a new 8.XX version of KiCad.

There are more possible combinations…but the question is when or whether the state of those 3 tick boxes is remembered.

5

I am not sure what is a big mess…

Right now I am dodging this issue by using only the footprints which are assigned in my symbol library and NOT changing that association in my schematic. I added symbols to my personal library in order to do this. But I would like to figure out what was going on. It is conceivable that it was all my fault, but this seems to be a new issue that I never encountered previously.

6

Actually for me the default setting of the tick boxes is Reiink: unchecked, Delete: checked, Replace: checked.

The Relink option is only needed for certain situations, it’s too early for me in the day to remember when to use it, but if it’s checked, then you would not be able to easily renumber RefDes on symbols, which I do a lot.

7

Thank you, retired cat…

So maybe once upon a time I checked that re-link box and it stayed checked. Maybe that was my big troublemaker. How long will it stay checked? Other than me unchecking it, are there any other operations (such as changing to a new project) which would cause it to become unchecked?

This is the reason for that question.

By the way, doesn’t a retired cat mean there must be such a thing as a cat with tires? Wheely? :crazy_face:

8

I did a little experiment. I toggled the Relink option, but didn’t update the layout. I exited the layout and schematic editors. Neither prompted me to save my work.

So I looked in the global KiCad preferences and the change appeared in the pcbnew.json file. This is the section that stores the options:

  "netlist": {
    "associate_by_ref_sch": false,
    "delete_extra_footprints": true,
    "delete_shorting_tracks": false,
    "report_filter": 29,
    "update_footprints": true
  },

So if you change those settings in one project, it will affect other projects you are working on.

Perhaps it’s a shortcoming that these options are not stored per-project.

9

Thanks a lot.

Just to be sure…I think that unchecking the first box means that linking is taking place via UUID and not ref designation. I have trouble keeping straight the ramifications of that…

Is it reasonable to say that the combination of first and third tick box is a bit dangerous?

So if I have changed a bunch of footprint assignments in my schematic, and now (without due care or some other way) update PCB from schematic with all boxes checked, now I will undo all of my footprint assignments made at the schematic level.

I think this deserves at least a warning or something? Especially since I might do it unintentionally, because I did it two months ago…

Is there one safest combination of tick marks to which it ought to default each time? Maybe another box saying “remember this setting”

10

Yes those are the two methods.

I’ll leave others to discuss the ramifications of the various settings or suggest reworking of the UI, it’s too early in the day for me to do any serious thinking, maybe even too early in the year.