How do I force a reload/refresh a part in schematic from lib

want to do the same as in layout

reload a certain part (all instances) with same part from library and sometimes with different part

how do do ?

Sometimes minor changes like the fields of a component goes unnoticed by eeschema and there is no option to avoid a rescue, the option is never raised.

As soon as you place a symbol (part) in a schematic the fields decouple from the library… this means you need to get your ducks in a row before that very moment (if you want atomic parts) or you have to live with it.

Things that will change when you edit the part in the library and save it there (don’t change it’s Value field as that’s the link):

  • symbol picture (lines, etc.) will follow lib
  • pin numbers/names/positions will follow lib

Things that won’t change:

  • any of the fields (content, positions, visibility, text sizes, etc…) are decoupled from lib

When you change the value field (essentially the part name/ID) in the library all bet’s are off as this will brake the link.


I know now that Value is the ID (should be Name instead of value IMHO :slight_smile: )

but not getting the fields updated is a pain
for example footprint is in the fields and a lot of other nitty gritty useful info (if you put it there)

Luckily for me I always used manufacturers part-no as Value, so no problem with that

but my other fields etc, ooooouuww

can i trick an update in by changing 1 pin name momentarily ?
would that provoke an update ?

it did not, i just tried

can i use search and replace in some text file ?

To get the symbol as far updated as possible (again, the fields won’t update ever afaik):

  • open the symbol editor (do NOT edit the part in the schematic)
  • navigate to the library/part and load it
  • edit the reference field by hitting [E] and mouse over (easiest imho), no change needed, cancel/OK action
  • save button becomes available (that’s what we want)
  • save part
  • go back to EEschema

Anything that didn’t change via this will never change and needs to be updated manually.

PS: yes, been there, done that… 4 PCBs made that way and survived to tell the tale… the 5th board is already started but this time I got my ducks in a row beforehand… just a hand full of connectors still to go and then I’m good and have everything set up to be atomic and keep making #5.

1 Like

KiField allows adding, removing and updating symbol fields (names and values but not size and position)


But not with the field values from the lib… it’s a more convenient (one-place) way to manually modify those fields.

1 Like

Yes, the only logical way.

Works nicely for footprints.
Exact same mechanism is missing.
And do away with the resecue mechanism.

But I look into kifields.

I see that Ki-fields can take fields from schematic into library

i wonder if the developer of ki-fields could fix it also the other way around

I dont know how to contact the developer,

is it you ?

I’d suggest searching for “KiField” on this forum :wink:

KiField can process symbol libraries too if that’s what you mean.

@nicholas needs a tool that loads the current fields from the libraries and updates the fields of the parts that have been placed in the schematic.
KiCAD doesn’t do that by itself. One has to manually update/edit the fields once the part is in the schematic - no way around that.
There is nothing like a “read netlist” button that would “update” the fields of the parts in the schematic with the content of the library, or is there?

KiField does allow exporting/importing of either library or schematic part fields to/from a CSV.
But it won’t help you “updating” parts in a schematic with field info from the libs.

Please correct me if I’m wrong.

Well, KiField can’t do it by itself but it can help: export fields from both schematic and symbol library to *.csv files, manually update schematic *.csv with data from the library *.csv using spreadsheet editor, import schematic *.csv into schematic.


Yes that will be my way forward.