Greetings -
I would like to consistently add a number of fields to every symbol property set. Its not important what they are but items like manufacturer, manufacturer catalog number, distributor, distributor catalog number. I would like to have this software-driven to avoid operator errors.
Is there a way to add to the default set, or to write a script to do this automatically when a new symbol is created? Oh, KiCad 6!
Many thanks
Jim Wagner
Oregon Research Electronics
Create a New Symbol then select the Icon shown and add your new fields during (or after) creation…
Try out the functionality of the field name templates. My hazy recollection is that when configured, those fields were also available to populate in the symbol editor. But AFAIR that was in KiCad v4 days and it may have changed. But since you are the one interested, why not do the experiment?
Because I am prone to “operator errors” with the keyboard, I am really looking for an automated way. Sure, I can add those manually in a variety of ways, including what BlackCoffee showed. That, however, does not satisfy my need.
Empty fields would go a small ways, but having the fields pre-named is important as that takes keyboard entry. Most of the fields can be filled using copy and paste from a manufacturer or distributor web site, but name usually takes keyboard entry.
Where do you find information about field name templates?
What I have started doing is manual creation of those fields in a part, say resistor, then copy and paste that part within the schematic. That helps, but it then gives you the sense of the new part properties all being filled in, making it easy to forget that new content is needed. And, you still have to get that first instance right. Maybe most of you don’t have keyboard problems or memory that works right every time, but not all of us are so blessed. Some help would really be appreciated!
Jim
My first choice would be to Create a New Symbol (example shows I named it “Default_1”.
It contains Fields I added during creation (as above)
Then, in the Symbol Editor, look in the Directory where you placed it and Right-click, Copy/paste or Save-As
Give it a new name then, tweak the fields as desired.
EDIT: Added… As far as Template’s: That Default I setup can be considered a reusable Template.
But, if want to know Where the Editable file is, look in your system for the file or, for specific projects’s schematic/symbol, edit the Schematic file with a TextEditor. Once file is found, it will list the Symbols and you can Edit the file (screenshot, and use your Speech-To-Text tools on your computer…
I’m amusing myself and pushing my neural connections…
If you like to program, you can create a Kicad Plugin or Stand-Alone app to Open the Symbol file or Schematic file and search for your custom Field(names) and Replace the desired Text. AND, do it All by Speech-To-Text.
I may play with this when temperature here (in Lake Oswego, OR) hits 90Âş today
But, for reference, if interested… I imagine just saying “Search Field 1” and “Replace Text1”
… got the idea…
Thanks, BlackCoffee -
I’ll go with some custom symbols such as cap_0805 with the fields added and named. That will go a long way because it will also solve symbols at obtuse locations such as “device” in the symbol library. That will solve two problems at once which is not all bad.
Yes, like to program. So, I may try a Kicad Plugin. Just down the interstate from you, near Corvallis. Hot here, also.
Thanks for the ideas,
Jim
These are in: Schematic Editor / Preferences / Preferences / Schematic Editor / Field Name Templates. Below I’ve entered three fields:
And then, when you edit the properties of any symbol on the schematic, these fields already “exist” for all symbols:
However When you open the Symbol Editor and open some schematic symbol, then these extra fields do not exits in the library symbol:
I do not know whether this is a feature or a bug.
Maybe they have just forgotton to add those “virtual” fields there too.
What do you mean with:
The “created” part, is that creating a new symbol in the library, or creating a new instance of a symbol on the schematic?
Thanks, Paul -
I tried but just could not find a template that dealt with symbol properties. That helps.
Either when creating a new symbol or a new instance of a symbol would work. My inclination would be to do it when the library symbol is created.
Best wishes
Jim
I use KiField (link, link) - A utility for manipulating part fields in KiCad schematic files or libraries. KiField can extract all the component fields from a schematic or library and place them into a spreadsheet for bulk editing, after which you can insert the edited values from the spreadsheet back into the schematic or library
Thanks, I’ll take a look at that. I find that populating part fields is one of the most error-prone elements of board design. Anything that will streamline that should be helpful.
Jim
Making the “Field name Template” fields also visible in the Symbol Editor has been an open issue for about 3 years now.
Jim,
Keep in mind that in KiCad symbol libraries, the symbol name and value fields are forced to be the same. 
Not sure why that was ever thought to be good idea, but it prevents you from making symbol libraries which are fully specified and ready to plunk down in the schematic (especially obvious with R’s, C’s, and L’s).
Here’s a discussion on this subject: https://forum.kicad.info/t/symbols-with-value-symbol-name-in-v6-0/35298/4
