[Solved] Easiest method to make resistor value visible in pcbnew

I sometimes construct relative large PCBs with 2 or 3 different resistor values. For these particular boards I am more interested in values than component numbers as it helps me solder faster.

The value is always in the F Fab layer by default. The first things I always turn off are the fabrication layers.

Is there an easier method to get these values in the front silk layer than manually doing that clicking work.


I can find the lines in the board files using regular expressions in VScode. And replace the texts bij hand. I do not yet know how I can let the regular expression ‘scipt’ can do this for me. I believe that should be possible.

\(fp_text value ".*R"


Besides such a script are there mores options in pcbnew to get resistor/capacitor values in the front silk layer? I am guessing that this ‘inconvenience’ comes from the component libary and therefor cannot be easily fixed like the the default text size?



@bask185 : Is there an easier method to get these values in the front silk layer than manually doing that clicking work.


  • right side appearance-panel: objects-tab, enable values, disable references, disable hidden text
  • right side appearance-panel: layers: enable fab-layer
  • optional: select DIM-display mode (this excludes all non-FAB-items from the forthcoming selection)
  • right side selection-filter: enable only text for selection
  • now select the value-strings on the pcb (or use CTRL-A to select all)
  • Edit–>Edit Text&graphics properties:
    • Scope: values
    • filters: only selected
    • action: Layer–> to F.silkscreen
    • action: text width/height/thickness: as desired
    • Apply & OK

note: this works for v6/v7. You shuld include the kicad-version in your thread-starting-questions.

note2: If you do this often/always: Maybe creating your own modified footprint-library is useful

Thanks it worked.

Wild numbers have appeared



1 Like

You can:

  1. Copy a resistor footprint to a personal / project specific library.
  2. Modify that footprint to have text in the orientation and layers you want.
  3. Use that modified footprint in your projects.

For existing projects, you have to modify the footprint links in the schematic and then update the PCB to use these modified footprints.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.