Hey all-

TLDR I just want to make text show up below the component footprint on the pcb to remind me which component type/value goes where when I solder the board without confusing the KiCad software.

For those more patient.... This should be super easy but I am having troubles... I originally tried naming all of the f.silkscreen component labels to their values IE (R12 to R500) for 500 ohm resistor. I had several of the same component name however and freerouter would not run so I then changed them to R500, R501, R502 etc and still could not run freerouter to make the traces as they now didn't match the schematic values. I went back to the schematic and changed and updated the board from the schematic to go back to the original labels and was able to route it. The issue is that it is very tedious when trying to solder the board to look back and see that R12 is a 100K and R1 is a 10K and keep them from getting mixed up with tiny smd components. I have tried to move the $REF labels to the f.fab layer using edit and edit text and graphics properties and then update the matching f.silkscreen to one with values now that it has been routed and it still auto updates and changes the $REF labels to match even though they are on different layers. It may not matter at this point but would rather not cause any undue issues. Any suggestions?



Thank you!

 

Why not just use the TEXT option on the front layer .just a separate label of your choice.?

 

I have tried to move the $REF labels to the f.fab layer using edit and edit text and graphics properties and then update the matching f.silkscreen to one with values now that it has been routed and it still auto updates and changes the $REF labels to match even though they are on different layers.

Suppose there's a component with reference field R1 and value field 100k. In the PCB layout editor, right-click the component, select "properties". Un-tick "show" for the reference field if you wish. Tick "show" for for the value field if not already ticked and make sure it's on the silkscreen layer that you want. I don't use freerouter and maybe I don't understand you issue.

 

you can create new field and call it something like Value2 and enter whatever you like.
i usually use this to specify component value that is shorter than manufacturer part number. then click on checkbox visible, set font size etc.


close the window, edit properties of just created label and change layer to silkscreen


now that you have things to your liking, you may want to save this footprint into your own library. this way, in the future, all you need to do is use this customized footprint and everything is already setup. you can change the footprint for all components of same format and they all will show their own value.

the advantage of doing something like this is that added field retains the tether to the footprint. this means even if you move this label away which happens a lot when arranging layout, you can find which label belongs to which part. same is if you change value in schematics, it will be updated on the silkscreen and BOM....
see the pink line from center of 1k to center ot R15 footprint? if not i added two yellow lines around it so it is easier to find.

 

example demo project Pic Programmer...
edit one of the footprints

place the value label where you want, such as center of the resistor box, perhaps make it stand out (italic, bold, whatever)


and then save it as a new footprint.



then replace all footprints on the board to use CUSTOM.
and you should get something like this


or this

 

Thanks all! Such a great forum...

 

the other thing i would recommend is to use interactive BOM plugin. it makes search for parts or references easy and shows where the parts are on the board (and the other way around)