Meaning of the layer names

[msauerpb]

Hi,
at the moment we use Eagle for layout pcbs but I’m evaluating the usage of KiCad. So I have a question about the layer setup. What is the meaning of the particular layer? E.g. courtyard, adhesive, fab, edge.cuts, …? Are the paste, silkscreen and mask layer the same is in Eagle? Are there a documentation which describes the layer functionality?
Thank you for your help.

BR
martin

[retiredfeline]

Just type in something like “what are the layers in a PCB” to a search engine. Really. I got a heap of hits. The layers are the same no matter what ECAD tool you use, but there may be small variations in naming.

[paulvdh]

Just as in any other PCB design suite, a lot of the layers have very specific meanings.

@msauerpb

Are the paste, silkscreen and mask layer the same is in Eagle?

Layer names are different, but their functions are very similar. I am not very familiar with Eagle, but there are differences. For example, some programs have layers reserved for copper zones, while KiCad combines both tracks and zones on a copper layer. When an Eagle project is imported in KiCad, KiCad can do an automatic mapping of eagle layers to KiCad layer names, but I am not sure how complete this is. Eagle appears to have many more (non functional?) layers then KiCad.

I had a look at the online documentation:

PCB Editor | 7.0 | English | Documentation | KiCad

(You probably also have a local copy of this document, it can be renered as html, epub or pdf) and I was a bit surprised it does not have a list of explaining the purpose of each layer in KiCad. The layer names are pretty much self explanatory though, and I guess most people working with KiCad for some time have forgotten how they learned the layer names

A short list. These are mapped directly to gerber layers:

• Layers ending in .Cu Copper layers.
• Adhesive is for glue dots to glue SMT parts to the PCB before soldering (common for wave soldering)
• Paste Mask for Solder paste. The solder stencil is made from this layer.
• Silkscreen a.k.a “Legend” for texts printed on the PCB.
• Mask Solder mask layers,
• Edge.Cuts is the outside perimeter of the PCB, it can also have extra cutouts and custom routing.
• Courtyard is for reserving space around parts and to make sure the parts can be placed on the PCB without overlaps or being too close to other parts.
• Fab Fabrication notes. For making documentation that is used during PCB assembly.
• User User layers are free to assign to anything you want.

I am not sure what the Margin layer is for. I looked a bit around on this forum and apparently other users are also confused by this. I did find another (old, KiCad V5) list of explanation of KiCad layer names:

What is the meaning of the layers in pcb_new and in the footprint editor? (KiCad 5 and earlier)

A pcb is a 3-dimensional object with different materials stacked on top of each other. If a designer talks about designing a 2 layer board then they typically mean that this board has two copper layers. A 4 layer board has 4 copper layers and so on. In addition to these copper layers there are other technical and documentation layers available. A good introductory read is this post by @dchisholm : Any way to make the screen more understandable? In KiCad the following layers are available. L…

[mf_ibfeew]

First cosmetic difference:
Eagle: top/bottom layers are differentiated by TOP/Bottom == t/b
kicad: top layers get F (Front), bottom layers get B (back) as letter.

In addition to pauls list here is a comparison between kicad layers ↔ eagle layers.
direct compatible layers:
F.Cu → Top (1)
IN1.Cu … In30.Cu → Route2…Route15 (inner layer copper)
B.Cu → Bot (16)
F.Adhesive/ B.Adhesive → tglue/bglue (35/36)
F.Paste / B.Paste → tCream/bCream (31/32)
F.Silkscreen / B.Silkscreen → tplace/bplace (21/22)
F.Mask / B.Mask → tstop/bstop (29/30)
Edge.Cuts → Dimension (20)
F.Fab / B.Fab → tdocu / bdocu (51/52)

user.drawings / user.comments / user.ECO1 / user.ECO2 / user.1 … user.9 → eagle layers > 53 → use them freely as you want

layers existing in eagle, but not available in kicad (due to different working principle):

• 17 Pads
• 18 Vias
• 19 ratsnest
• 21/22 torigin/borigin
• 25/26 tnames/bnames
• 27/28 tvalues/bvalues
• 33/34 tfinish/bfinish
• 37/38 tTest/bTest
• 39 / 40 tKeepout / bKeepout : partly use courtyard around ffotprints, partly use rule areas
• 41 / 42 / 43 Restrict areas: instead of layers this is implemented with rule area item
• 44 / 45 drills / holes
• 46 milling use: use graphic shape on edge.cuts (dimension) instead
• 47 measires: use meaurement-items instead and place on every desired layer
• 48 Document: use oe of the generic user-layers (user.drawings / user.comments)
• 49 Reference

layers existing in kicad, but with no exact representation in eagle:

• F.Courtyard / B.Courtyard: is drawn around all footprints and allows to prevent footprint-collisions. A little bit like the tkeepout/bkeepout rectangles around footprints in eagle.
• margin: works like a dimension-item in regard of clearances, but without a real milling/drilling. Can be used for easy/fast keepout on all layers.

[paulvdh]

Some of the things that appear to be separate layers in eagle (such as pads, via’s, References) are handled via the Appearance Manager / Objects in KiCad.