Gerber generation ".Fab" Layer

Hi All

When generating the Gerber files for the “.Fab” layer is there a way of switching off the Values of the components so that the output for the layer is just the component outlines and references.


I am looking for an output similar to this screenshot from PCBNew.

However I get this. The Values of the components add more information I don’t need.

Hmm? I never had to do this because the outlines and references are already on the *.SilkS layers. So I just don’t generate *.Fab. What do you use *.Fab for?

I also use the .*Silk layer for the moment. It’s just that the .*Fab layer looks neat. So I was considering switching and using it for my Assembly Drawings. Unfortunately the issue above is holding me back :grinning:.

You can still remove the information you don’t need. When you create a footprint, don’t include the information you don’t need. You decide what is on the F.Fab layer, KiCad won’t stop you from using it for what you want.

You can set them to hidden. Double click on the value and disable “Visible”. Hidden values are not exported when creating Gerber, PDF, SVG or any other graphical export files.

I understand that this would solve the problem. I could do it for a small board with a few components. However it becomes labour intensive for higher number of components. I thought there was a quick way to hide all from the Gerber file.

Thanks for the suggestion.

Do you use your own footprints or do you use the footprints provided from KiCad? If you use your own, you can set them to hidden in the library and then update the footprints from the library. In Pcbnew under Tool -> Update footprints from Library … and set “Reset text layers and visibilities”. This way you only have to change it once per footprint type and not for each component that uses the same footprint. But it will reset all text from all footprints.

Or you could use the Python API when you have some programming experience.

1 Like

I’ll try this. Thanks.

For the Python approach: Open the Python console in Tools -> Scripting Console and enter the following text:

import pcbnew as p
for m in b.GetModules():

After that all Values should be hidden. This is probably a safer approach than changing it in the library and updating the footprints, because this way nothing else changes.

1 Like

I appreciate. Thank you.

It worked, perfectly. :clap: :clap: :clap:

Which layers show that screenshot (the black one from Pcbnew)? F.Fab or F.SilkS? If it is the later, make sure you don’t export the silkscreen over the pads.

Edit: Sorry, false alarm. I was confused by the fact that the values where not shown in Pcbnew. I forgot about the Values visibility settings in the Layers Manager tab Items.

1 Like

This is from the .*Fab layer.

In File-Plot you have check-boxes “Plot footprint values” and “Plot footprint references” that allow you to switch them on/off separately.
The question how to get documentation files I need was my first before I started to use KiCad.
We used to do two pictures. One with element rectangles and values inside (black) against copper layer (gray) and second with element rectangles and references inside against copper layer. When I search a problem in PCB I use picture with values (I don’t care if it is R7 or R25) but I need to know what is its value.
To not have the numbers too small I prefer the biggest possible rectangle so I decided to use CrtYd layers for it. I use only my own libraries.
At the beginning I wanted to use File-Export-SVG. As there are no check-boxes for hiding values and references I had to use separate layers for them so I used Silk and CrtYd. Then I changed my mind few times.
Why I now don’t use Silk for it?
At Silk I mark pin 1 that way to avoid pads. At CrtYd I mark pin 1 to be easily seen at picture ignoring pads. So as CrtYd goes to my picture if value and ref are there it is just simpler.

1 Like

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