Editing one property of multiple footprints

Software
1

I’m looking for a way to edit one property of a number of footprints.

For example, I have a number of components on my board which will not be populated but are there as a backup (things like a simple PI-filter, a 3 resistor attenuator,…)

When you add components to a schematic or footprint Kicad always displays both the reference designator and the value as part of the silkscreen.

Is there a way to select a range of components and set the property of the silkscreen to ‘Invisible’? Right now I have to edit each footprint, edit the value, put ‘Display’ to ‘Invisible’ and click OK two times.

There must be an easier way to do this?

2

What version of Kicad you’re using?

The fastest way I see is to edit the pcb as a text file and add “hide” modifier after the object you’d like to make invisible. As an example, here is a snippet of a .kicad_pcb file from my recent project, you’ll see the “hide” modifiers on reference and value fields there:

<...>
(module Pin_Headers:Pin_Header_Straight_1x02 (layer F.Cu) (tedit 543AD1B5) (tstamp 54396419)
(at 144.145 104.775 90)
(descr "1 pin")
(tags "CONN DEV")
(path /53E52E0F)
(fp_text reference P1 (at 0 -2.286 90) (layer F.SilkS) hide
    (effects (font (size 1.27 1.27) (thickness 0.2032)))
)
(fp_text value IN (at 0 0 90) (layer F.SilkS) hide
  (effects (font (size 1.27 1.27) (thickness 0.2032)))
)
(fp_line (start 0 -1.27) (end 0 1.27) (layer F.SilkS) (width 0.254))
<...>
3

Currently I’m using version BZR 5161 from 2nd of October 2014.
Quite recent…

Indeed, editing these properties in the text file mode is a possible way
forward.
But more interestingly I would like to see if I could manage this from the
scripting console.

Perhaps there is een API available to work on components?

Is there already a feature request for such a property editor? Otherwise
I’d add it to the Launchpad in the hopes it receives some more attention.

4

Hi tipofthesword,
Realise this is an old post, but a script to do what you want appears reasonably straightforward. The script below tests fine, presuming you know the references of the parts you’re wanting to change.

#!/usr/bin/env python

from pcbnew import *
pcb = GetBoard()
while True:
    thing = raw_input('Reference to hide: ')
    aModule = pcb.FindModuleByReference(thing)
    if aModule:
        aModule.Reference().SetVisible(0)
        aModule.Value().SetVisible(0)
        print('Module '+aModule.Reference().GetText()+': '+aModule.Value().GetText()+' is now hidden.')
    else:
        print('Module '+thing+' not found.')    
    again = raw_input('More? Y/N: ')
    if (again != 'y') & (again != 'Y'):
        break;
print('Done.')

References are case sensitive, so c1 is not the same as C1. This hides the reference and value in the currently open board in pcbnew.

Cheers! Geoff

1 Like
5

This is an old thread, but thought I would throw this out there. I updated a bunch of footprints and needed to hide all the “value” fields as mentioned above. I opened the pcb file in Vim and ran a one-liner:

%s/^.* value .*)$/& hide

This could be done with Sed also, and changing “value” to “value 10uF” lets you be more selective. The power of KiCAD’s human readable file formats.

2 Likes
6

And then there is this here:

Currently going over @devbisme’s KiField code to see how this is done more properly than I do in my ugly code.
Should have an option to export the settings from CSV back into the kicad_mod repos in a couple of days/weeks.

7

A post was split to a new topic

8