Looking for info - layer names

I’m trying to find info of what each layer is, or rather descriptions to what each name means.

I got the B back side and F front side, and some others, but a cheat sheet could really help…


Here is a link to the documentation that @Andy_P mentions:

In summary:

  • Between 2 and 32 copper layers for routing tracks. These are the layers with configurable name.
  • 14 fixed-purpose technical layers:
    • Layers that come in pairs (Front/Back): Adhesives, Solder Paste, Silk Screen, Solder Mask, Courtyard (undocumented yet), Fab (undocumented yet)
    • Standalone layers: Edge Cuts (board outline), Margin (undocumented yet)
  • 4 auxiliary layers that you can use any way you want: Comments, E.C.O. 1, E.C.O. 2, Drawings

I’ll try to update the documentation.


Good stuff, just what I was looking for.


Just to note:
None of those have the Front/Back feature… so if you place something on one of those layers in the footprint editor (you can’t directly draw on those, but the [E]dit option let’s you move drawings onto those layers) and you flip the footprint, those layers won’t flip.

Also, just in case someone needs it and stumbles across this… If you need more than one reference and/or value field to appear (for example for documentation purposes you might want to have REF on F.Silk and also on F.Fab) you can make Text fields on any layer you want and use %R for reference and %V for value.

1 Like

See atch for a sample of the kinds of information I typically put on “Drawings.User”. This example is a pretty simple board, and still in progress. The dimensioning is more important when the shape isn’t a simple rectangle. I often include outlines and mounting hole locations for large components like power transistors, and connectors or switches or other things that must interface mechanically with other parts of the final product. If space permits, I try to include a generic illustration defining max length for component leads and solder fillet on the back side of the board. It’s useful to print this layer 1:1 as a crude visual check when naked boards are received, to be sure the shape is correct (e.g., a slot didn’t get accidentally moved to its mirror image location), mounting hole locations and sizes are correct, etc. The 1:1 printout is also useful for creating physical mockups, laying out test fixtures and assembly jigs, etc.

I struggled with this a few months ago and finally decided that it couldn’t be done. Now, if only my superannuated brain can just remember this post the next time I try to include values or ref des on some ancillary layer. Sounds like another topic for the sub-section in my imaginary manual called something like, “Features, Capabilities, and Conventions Related to Text in KiCAD (That May Not Be Intuitively Obvious to Mere Mortals)”.

Dale Clk_Ctrlr_B-Dwgs.User.pdf (71.2 KB)

1 Like

this, so much this :heart_eyes:

Lol… me toooo.
Final straw was me posting on the launchpad question list - if there was a way to get those fields onto another layer and the reply was so astonishingly simple, I just couldn’t believe it at first :open_mouth:

R_0805.kicad_mod (1.4 KB)

With different color-layer assignments and switching layers on/off I can have some easily visible reference field during layout that doesn’t disturb my view and also some big enough reference/value fields later on for documentation:

PS: that pdf looks really smooth, hat’s off to you sir.