Do I have to edit every pad individually to enable F.Paste technical layer for stencil

Layout
1

After finishing my PCB layout I generated the F.Paste gerber for a stencil and it was empty. After some poking around I discovered that the F.Paste technical layer was unchecked on every SMD pad. To fix this I had to edit every pad and enable the F.Paste layer, as you can imagine this took a while.

Is there a better way to do this? It seems odd that F.Paste would be disabled by default.

2

What OS?
What KiCAD version?
What library/footprint repo did you use?

3

@SchrodingersGat
How is the feeling of the library maintainers about this?

Currently the only thing the kicad library convention states about layers is the following:
KLCv1.1: Silkscreen is not superposed to pads
KLCv1.2: Pads should not have Silkscreen layer enabled
It is not even mentioned that the mask layer should be enabled.

Edit: I just checked a few of the kicad official libraries and they seem to have the paste layer enabled.
I checked the what the setting is in the python footprint generator script and i checked the smd buttons library.
I still think stuff like that should be mentioned in the KLC

4

This has been added to the draft KLC here: https://github.com/SchrodingersGat/kicad-library/wiki/KLC

5

the new klc already seperates tht and smd footprints. maybe the pad layers should be defined a bit better.
But as i said above i did not find footprints (yet) without paste layer.

@MarkOsborne: what footprints don’t have the paste layer activated?
We can only help/ change the kicad official footprints. If you got them from somewhere else contact the people who made these footprints.

By the way you don’t need to edit every pad on the pcb. But you need to edit every pad in every used footprint.
After that you need to update the footprints on the board by opening the properties of one footprint and than go to change footprint.
In this new window select all footprints on the board and press apply

6
  1. Edit kicad_pcb file with good plain text editor and add F.Paste or B.Paste for each SMD pads. Maybe better than clicking but still time consuming and error prone.
  2. Write and run Python script to enable paste mask for each SMD pads on board. Black magic for non-programmers.
  3. Edit footprints in used libraries and enable paste mask for each SMD pad once, then replace footprints by Exchange footprints command. If you have these libraries on your drive or have got full access to them.

If you have Python programming skills select 2, but if you want to resolve this issue once for all time, select 3.

1 Like
7

I was seeing the problem with standard kicad libraries. e.g. Capacitors_SMD:C_0805.
However, if I open the original parts from the kicad libraries in PCB Footprint editor, I see that the paste layer is enabled!
Which leads me to think that it was something that I did wrong initially - this is my first Kicad board.
I tried creating a new board from scratch and everything worked fine!

Thanks for your responses, I’m glad to know that paste would normally be enabled by default.