Tip to equip symbols with additional fields

[Lutz_Muller]

Hello everyone, I have just added additional fields (row and column) to all symbols.
For this I used Notpad++. After setting the formatting to Assembler under Language, press Ctrl+H. Now set Find regular expressions at the bottom left. (1)

When searching, enter the regular expression to search for:

^(\s+(property "Datasheet" "" (at [\d.]+ [\d.]+ [\d.]+)\s+(effects (font (size [\d.]+ [\d.]+)) hide)\s+))

This looks for the following text block:

(property "Datasheet" "" (at 12.065 11.43 0)
  (effects (font (size 1.27 1.27)) hide)
)

The same applies now to the text to be replaced:

$1\r (property “Zeile” “” (at 0 0 0)\r (effects (font (size 1.27 1.27)) hide)\r )\r (property “Spalte” “” (at 0 0 0)\r (effects (font (size 1.27 1.27)) hide)\r )

This is the result:

(property "Datasheet" "" (at 12.065 11.43 0)
  (effects (font (size 1.27 1.27)) hide)
)
(property "Zeile" "" (at 0 0 0)
  (effects (font (size 1.27 1.27)) hide)
)
(property "Spalte" "" (at 0 0 0)
  (effects (font (size 1.27 1.27)) hide)
)

For a line break, insert \r.
Before each bracket you put a \, examples: \(, \).

[devbisme]

I think you could also do this with KiField.

[paulvdh]

What is your reason for wanting to do this?
As long as those fields are just empty, it is probably better to use Schematic Editor / File / Schematic Setup / General / Field Name Templates. In that location you can define “virtual” names, that appear in every schematic symbol, and when you add data to the fields, they become “real”.

[Lutz_Muller]

Kannst du mir ein Foto machen? Die Übersetzung ins Deutsche verstehe ich nicht.
Habe gerade wieder vergessen den Übersetzer zu benutzen.
Can you take me a photo? I don’t understand the translation into German.
I just forgot to use the translator again.
I do this to give all symbols these fields.

[paulvdh]

And then the properties of a standard, unmodified resistor:

[Lutz_Muller]

I just learned something new. It’s amazing how much KiCad can do. Actually, I should now write an instruction manual on how to create a circuit diagram in KiCad.
But I have one more question before I start. Can I somehow hide all the network identifiers at once, or better yet, color them wisely so that you can’t see them right away?

[mf_ibfeew]

You could try the tool: main menu bar–>Edit–>Edit Text and graphics properties

In the top left you could restrict the scope to only affect labels.
In the top right you could restrict the scope to affect all schematics or only selected parts.
In the bottom part you could choose the new label size/label color.

Simple hiding the labels is not possible, there is no layer manager / item appearance panel in the schematic editor.

[Lutz_Muller]

The first picture shows the order of how to make the labels white so that you can’t see them after printing.

And the second picture shows how to restore the caption.