← Back to team overview

kicad-developers team mailing list archive

Re: PROPOSAL. Pcbnew anf GerbView layer names - can we improve them?


On Wed, Apr 10, 2013 at 04:16:50PM +0200, Fabrizio Tappero wrote:
> Hello,
> After a quick hystory check I noticed that in PCBNew (and in GerbView)
> and maybe in other places, the names for layers has changed quite a
> bit. Since I personally find (no offence) current naming a little
> short I'd like to propose some changes. Please forgive me if I am
> saying something stupid.
> So here it goes, nn the left the current names and on the right my
> propositions. At the bottom I also would like to propose some minor
> name changes, please comment if you like.
> Copper Layers      ->  Signal Layers
> F.Cu                    ->  Top Copper
> B.Cu                    ->  Bottom Copper
> Inner1.Cu             -> Mid Copper 1
> Inner2.Cu             -> Mid Copper 2

Inner is the world wide standard. NOBODY calls them 'mid layers'; Front
or back, top or bottom are the same, some standard use 'primary' and
'secondary' other simply call them side 1 or side 2. Historic names are
also hot and cold (since had soldering only on the bottom side). And
anyway the name of the copper layer is customizable *at the board
level*. The component editor uses the default names (since it doesn't
actually know the board) and the plotter at the moment is using the
default names too (there was a discussion about this a while ago, IIRC;
that would be open to suggestion, but anyway the script interface use
whatever name you want).

Also I'm tired of these changing layer names, that would be maybe the
fourth time since I started using kicad...

> Technical Layers    -> Non-copper Layers (or Mechanical Layers or
> Non-signal Layers)
> F.Adhes                 -> Top Adhesive
> B.Adhes                 -> Bottom Adhesive
> F.Paste                 -> Top Solder Paste
> B.Paste                 -> Bottom Solder Paste
> F.SilkS                 -> Top Silkscreen
> B.SilkS                 -> Bottom Silkscreen
> F.Mask                 -> Top Solder Mask
> B.Mask                 -> Bottom Solder Mask
> Dwgs.User             -> Drawings
> Cmts.User                 -> Comments
> Eco1.User                 -> Extra 1
> Eco2.User                 -> Extra 2
> Edge.Cuts                 -> Edges

Uhmm these are more or less the old names IIRC... the Eco could be
happily renamed to Extra without problem.

Actually we have different kind of layers in pcbnew (I looked over layer
usage for MONTHS and I'm a self designated expert on the field):

- Copper layers (front, back and up to 14 in between). Front and back
  are flippable.

- Technical layers: paste, silk and mask; All of these are flippable
  *and* have special handling (clearances and stuff). Adhesive is more
  a comment layer, it has no special handling.

- Comment layers: these have no special function whatsoever: drawing,
  comments eco1 and eco2 are totally interchangeable for what they do...
  adhesive is actually a comment layer but it's flippable (the other
  ones are not)

- The all-powerful master edge layer which actually influence the other
  ones (the One-Layer!). Nominally alignment targets reside here.

Copper layer are already renameable. This is useful since often internal
layers are used as power plane.

Technical layer and the edge layer are very special (they have
behaviour) so they should not be renamed.

Comments layer could be actually usefully renamed (for example I often
use the comment layer for mixed voltage clearance markings, and a rename
would be fit). At the moment, the only 'flippable' comment layer is the
adhesive one.

Also there is the issue of modules: they live detached from the board,
yet the layer set is the same. That would give problem when mixing layer
conventions. I.e. a drawitem in a module 'comment' would appear on
whatever layer the designer is using the comment layer for.

Scheduled for addition (when even libs are in the new format):

- Courtyard (flippable)

- Assembly (flippable), also with a rule to put the reference on the
  origin of the component, when plotted on the corresponding layer.
  Explanation: when you have tight components you often move all the
  reference on a side (maybe drawing an arrow or bracket); on the
  assembly drawing instead the reference should be on the drop site to
  verify the placing program. Also assembly usually contains
  manufacturing comments.

- What else? the suggestion box is open.
> These changes will also imply the following changes:

I don't see any implication relationship; anyway...

> Through Via       -> Through Vias
> Bl/Burried Via     -> Blind/Burried Vias

It's buried with only one 'r' :D

> Micro Via           -> Micro Vias
> Pads Front         -> Top Pads
> Pads Back         -> Bottom Pads
> Text Front          -> Top Text
> Text Back          -> Bottom Text
> No-Connects      -> Unconnected

You should call them Unconnected Pads, to be coherent...
From an usability standpoint having 'Pads Front' instead of 'Front Pads'
give me a slightly faster eye scan. However I usually just look for the
color swatch, rarely I have to read the whole text (I could actually use
a layer 'strip' with only tooltips, after the first two days on a board
I guarantee you that you remember them without looking:D)

> Modules Front    -> Top Components
> Modules Back    -> Bottom Components
> Values               -> Footprint Values
> References        - Footprint Names

Kicad vocabulary: components are instances from the netlist, modules or
footprints are the pads and drawitems that implements them. So it
actually would be the other way around (component value/reference and
module top/bottom pads). Data dictionary nitpicking:P

> Here few questions to who knows the answers:
> 1) why is now a top layer named "Front Layer" and not "Top Layer". I
> guess the anwer has to do with the "Select Layer Pair" Menu. I think
> this menu can still stay.... even though I do not really see its use.

As I said it's only a personal habit convenience. No idea about who decided to
change. From the CAD perspective is the 'front', from a manufacturing
perspective it's the 'top'. Nothing change, really.

> 1) Applying these names the PCBNew "Layer Manager Toolbar" which maybe
> should be called "Layer Manager" becomes larger and this might upset
> Kicad mobile phone users. To satisfy them too, I'd like to propose a
> smaller font and padding for it. This will maybe take up just few
> pixels more than the current solution.

ARE YOU JOKING RIGHT?!? Just now it doesn't even fit in a 1024x768
screen, don't even think about phones :D

Also please take advantage of environment preferences, 1920x1080 at the
current size is a little small for me (I have powerful glasses :D), yet
the current toolbars don't fit in a 1024x768 screen. But maybe wx or gtk
is to blame...

Lorenzo Marcantonio
Logos Srl

Attachment: smime.p7s
Description: S/MIME cryptographic signature

Follow ups