Change the font size to multiple footprints at once?

Layout
1

Hi!

when the pcb is too populated with smd components it’s a bit annoying to change the size on every reference one by one, Is there a way to change all of them to a size and thickness?

2

Not directly via the graphical interface. (At least not that i am aware off.)
You could look if there is a script for that or write your own.
Another alternative is using a text editor. (The pcb file is human readable.)

For both workarounds: Make a backup beforehand in case something goes wrong.

3

maybe it’s the time to begin to use some python there then :slight_smile:

4

You could use a script like this :slight_smile:

import sys
from pcbnew import *

"""
execfile ("c:/python_progs/test_pcb/set_text.py")
"""

def SetText(Filename = None):
    if Filename: 
        my_board = pcbnew.LoadBoard (Filename)
    else:
        my_board = pcbnew.GetBoard()

    for module in my_board.GetModules():
        print ("module ref %s %s" % ( module.GetReference(), my_board.GetLayerName(module.Reference().GetLayer())))

        # set size in mm
        module.Reference().SetSize (wxSize (FromMM(2),FromMM(2)))
        
        # set thickness in mm
        module.Reference().SetThickness (FromMM(0.3))


# SetText("C:\\git_bobc\\bobc_hardware_live\\Smart_RGB_LED_AT85\\rgb_led.kicad_pcb")
SetText()
5

Great, I just need to learn how to use it! (never used a python script on kicad, until now)

6

The way I do it :

To run from kiCad script console in pcbnew

  1. Open the console, Tools->Scripting Console
  2. type the following command in the console window

execfile (“c:/python_progs/test_pcb/set_text.py”)

change “c:/python_progs/test_pcb/” to where you stored “set_text.py”.

When v5 is out, it will be much easier to run scripts.

7

In recent Nightly builds there IS a native tool for this. In PCBNew’s “Edit” drop-down, select “Set Footprint Field Sizes”. You can then set global values for the Reference Designators, the Values, and the User Defined fields. The new values persist if you re-import the netlist, too!

722×637 93.9 KB

756×437 44.6 KB

Dale

6 Likes
8

oh, yes, I saw that before (I have the heikkipu version with tears and curves, not the latest but close), however I believed it may be not working, because I fail to selected where to apply the new dimensions (this step was no self evident for me at the first time). Now I have it!
BTW bobc: how one run scripts in V5? (so easy, I can’t find it - I also compiled the last, just in case, but can’t find it anyway)

9

v5 is not even close to being released. (Currently it looks like it might take until next year.) Nightly is a development build! (Just a pre compiled version of the current git master branch.)
Fair warning: The nightly version is not meant for production. It is not guaranteed that files generated by a specific nightly build can be opened by either the stable build or older nightly build versions.

I think this is what @bobc was referring to.

10

my bad, since I not using the pre compiled (nightly) but V5 version (when I use the V5, not all the time) made by heikkipu (https://github.com/heikkipu/kicad-devel) just because I like the curves/tears.
I’m compiling this version and didn’t add the option of scripting when configure, I just need to read a bit further the install procedure to see how to turn KICAD_SCRIPTING=OFF to ON
This is why I didn’t have scripting console here!
I have the nightly in other partition to not mess with the V4.0.7 install, I went there and see the scripting console still exist.

11

Not only in nightlies. This tool hass been present from some years now.

1 Like