I'm fairly new to PCB designing, and it's my first board design.

If I want to add pin number silkscreen on the board, do I have to do it all manually on the board design page?

Can't I do it on schematic design page and pass it over to board page? Like putting labels on connections and make Eagle automatically show labels on silkscreen layer.

Any help would be appreciated.

  • 2
    \$\begingroup\$ Can't do it in the schematic design page, but if you edit the part library package you can put them in there. \$\endgroup\$
    – awjlogan
    Jun 7, 2018 at 9:29
  • \$\begingroup\$ hmm, I was hoping I could add some kind of text to the pins, and they would be passed to board design page. Thanks :) \$\endgroup\$
    – angrypig7
    Jun 7, 2018 at 11:10

3 Answers 3


The industry standard is to place a pin one indicator when you make the PCB footprint or to make pin 1 square and the others round. Anything beyond that you add manually to the PCB.

I personally don't annotate the schematic. However I find adding the actual signal names to the bottom silkscreen a lot more informative than the pins numbers:
enter image description here
(Company name has been removed) You can also see that pin 1 has a square solder mask, the others have a round solder mask.

If you work in a company with a PCB lay-out team you normally have to give a lot of instructions when you hand over the design. Those can contain anything from detailed component placement to what should be on the bottom and top silkscreen.


You can add the pin numbering in the footprint of you component. This is how usually this thing is done. In this way, each time you add your connector in the schematics you get the desired pin numbering in the board.


As RodezIO mentioned, you can do it in the footprint of the part, however, if you need some custom text, and repeated text(This is purely for the silkscreen):

You need to add an attribute to the 'tNames' layer that is assigned to each part. And convert the existing 'tNames' layer stuff to the 'tValues' layer.

Note that this is per part attribution, and not per pin.

For example, in the schematic:

  1. Select a part, then click on 'define attributes'> 'attribute' 


  1. Put the Name field: PIN_1 (This is unique per part)

3. Put the Value field: GND (input the name you want to write for each pin here. The same name can be repeated for multiple pins)

4. Put the display field: value

  1. you can add more attributes and follow the above steps.

  2. click ok and ok


  1. Click on the generated attribute field, and edit its font, style, etc.


  1. Resize and reposition it in the schematic

  2. Generate the board file.


  1. Click on the component name in the attribute name on the board file and change it to layer '25 tNames'

25 tNames

  1. Change the value of the pin(P1, P2, etc) to the layer '27 tValues'

27 tValues

  1. When you generate the preview or the 3d part, the silkscreen will generate with the 'GND' name and not the value

3d pcb

The default name attribute (in this case J1) could not be changed. Hence, I have pushed it to the 'tValues layer' and pulled the other attributes on the 'tNames' layer.


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.