I'm a music electronics hobbyist, and am in the processes of switching from Eagle to KiCad.

For some components — particularly potentiometers — it doesn't make sense for the name/reference property to be numbered. As it stands, though, if I name the volume pot "VOLUME" KiCad insists on renaming it "VOLUME1" before checking rules, generating netlists, or exporting to Pcbnew.

It's a pain to undo the numbering and edit the references on the PCB silks.

Is there some setting I can't seem to find to prevent this, or some other best practice?

  • \$\begingroup\$ For that part make the component name invisible and add a new property to the part called "volume". Make "volume" visible on the silk screen layer. \$\endgroup\$
    – Andy aka
    Jul 1, 2020 at 15:20

2 Answers 2


Take the part numbered at Volume1, in PCBNew when the component is where you want it, right click the part, open properties, untick show for the reference, and then press the "+" circled in the below image to add a new field with whatever text you want,

This is my preferred method, as the reference follows the part if I move it later, compared to just creating a text string on the PCB.

enter image description here

  • \$\begingroup\$ got it, thanks! it's a shame that there's not a way for you to add this property in the footprint editor directly, instead of having to do it manually for each component duing layout. would be cool if the footprint it can "inherit" custom fields from the symbol editor for certain components like pots and switches... oh well! :) \$\endgroup\$
    – burr
    Jul 5, 2020 at 23:44
  • \$\begingroup\$ You can bring custom fields from the schematic symbol into the PCB. In the schematic editor, open the Symbol Properties and add a field - give it a name like Label and fill in whatever you want into the value. In the PCB editor, open the Footprint Properties and add a text item with the contents ${Label}, make sure Show is ticked and it's on the right layer, and it should show up once you close the properties box. You can also add that text in the footprint editor. \$\endgroup\$
    – sandyscott
    Apr 28, 2023 at 12:06

Every part needs to have a unique identifier, usually called the "reference desginator", so that you can account for it correctly in the BOM (bill of materials).

You should not try to use the reference designator as a functional label (what if you have more than one of the same function in the design?) — instead, you should create a new property field for the part and use that in the silkscreen, assembly drawing, etc. in place of the reference designator.

  • \$\begingroup\$ Thanks! so you mean... in the Symbol Editor, add a new field to the component, like "Function" or something, and make that visible instead of the "Reference" field? OK, I see how to do that for Eeschema. How does one make this new field accessible in the Footprint Editor? \$\endgroup\$
    – burr
    Jul 1, 2020 at 15:54
  • \$\begingroup\$ I'm fairly new to Kicad myself. Hopefully, someone else will be able to give you the details. \$\endgroup\$
    – Dave Tweed
    Jul 1, 2020 at 15:56
  • \$\begingroup\$ The current version of kicad does not support using any other symbol field than value or reference in the layout. However you can just add a manual text field on silk to add user readable text. \$\endgroup\$ Jul 3, 2020 at 16:07

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.