kicad-developers team mailing list archive

[Lorenzo Marcantonio <l.marcantonio@xxxxxxxxxxxx>]

On Wed, Sep 10, 2014 at 01:41:33PM -0400, Wayne Stambaugh wrote:
> Perhaps we should define the layer behavior for footprint text and
> non-footprint text first and then make the code match the behavior.  It
> seems to me once you have the behavior defined, the code should be
> fairly straight forward.  I guess the real question is do we want to
> keep the current text layer behavior or do we want to design something
> that is more flexible?

I think that the reason behind having reference/values independant from
the silk layer is that often a thick silk hide the trackage so it would
be disabled during routing. However the reference is still useful in
orientating around the board so it's possible to have silk hidden and
references shown. Value behaviour is probably the same for uniformity.
Charras could probably shed more light on that quirk. Anyway I find that
behaviour useful.

The behaviour which we are discussing however is contained in the
collector and in the draw routine, so it's not too difficult to change.
I have this assumption that user module text contains nothing too
important for the normal routing i.e. is documentation and drawing
stuff. Feel free to give a counterexample of course; I have none.
Polarity is usually obvious from the pin name. Also my workflow has all
the 'needed' layers on during placement (silk, courtyard, comments for
keepout and so on) and most stuff disabled during route (I usually keep
assembly or silk on for orientation).

As a working case let's say I have some kind of backward mount
potentiometer (the ones you screw on the board and then solder) which
has maybe some important 'take care' area (maybe for the shaft nut or
something like that). Well, I would actually put a huge supporting
copper pad for the nut, but imagine I simply want to draw a comment (to
some pair of layers F_Comment and B_Comment) to remember that is a bad
place to route stuff for ESD or whatever. That's would be quite complex
component to draw, place and route around. It would contain:

- Pads and the big hole for screwing the thing on

- On the 'front' side (where the body will be): silk for the body,
  courtyard, assembly outline, comment outline; there will be the
  mandatory reference/value fields on F_SilkS (value always hidden with
  the flag), the assembly label on F_Fab (with the to-be-implemented %R
  token) and some text saying "Be Careful Here" inside the comment area.
  Also some other text on F_SilkS to remember which wire goes where.

- On the 'back' side (where the shaft would stick out): courtyard for
  the nut, comment outline for the corresponding area; some text on 
  B_Comment saying "Careful Here, too"

To keep things simple let's say it's placed on the top side (so I'm
seeing the bottom of the pot can and the shaft sticks under the board).

The behaviour which I am implementing is as follows (as usual all
condition are and-ed; if one fails text isn't shown):

- The root of everything is the module, of course; if the modules
  front/back visible is disabled nothing is show for a module placed on
  that side (even if the text would come up on the other side);
  I sometimes would have found useful to selectively hide some module
  but that's another enhancement:P

- Then comes the text front/back visibles: they operate on all the texts
  on that side: so the "text back" would operate on the "Careful Here,
  too" text, while the "text front" on the reference, value, assembly
  label, wire silks and "Be Careful Here"

- At this point the rule is different for reference/value/user text:
  - Reference is controlled by the "References" visible, and takes color
    from the "Text Front" visible (since the module is on the front
    side)
  - Value is the same but controlled by the "Values" visible
  - User text is controlled by the corresponding layer control, both in
    visibility and color

- The last thing is the 'hidden' flag in the text itself; if set the
  text is only visible if the "Hidden Text" visible is set (and takes
  that color);

For example the value would be visible (in Hidden Text color) only when
"Hidden Text", "Text Front" and "Module Front" are enabled. That's
*exactly* how pcbnew works today.

In the same way the "Careful Here, too" text would be shown (in
B_Comment color) only when "Module Front","Text Back" and the B_Comment
layer are enabled.

Philosophical experiment of me routing that component:

Now, let's say I've already placed the thing (with all the layers and
stuff enabled) and I go routing. The silk screen isn't really useful for
orientation since it's only a partial outline, so I turn it off. And the
wire labels disappear; no panic, I have the netlist anyway, that's meant
for the people assembling the board. Even disabling silk the reference
is still shown since it's a special field. So I can still see the name
of what I'm looking at. For orientation it's more useful the assembly
layer (which now has its own label). That's controlled by the assembly
layer control. Turn it on, assembly outline and label appears; turn it
off, both disappears. Also there is still probably the reference on the
screen, probably conflicting with it (they often start overlapped since
you don't know in the librarian where/if there is place for the refdes
on the board). Hate when that happens, can't read any of them! I can
turn off all the references without problem however. Since I can see the
assembly labels I don't lose my way on the board.

So, first consideration: the 'real' reference attached to the component
is the one on the assembly, the one inside it. Our reference (that goes
on the silk) has to be placed outside or even hidden (if there is no
place for it) so it's not so useful during routing. However we can't
change that because it would break older files... the mandatory
reference has to be the one on silk (accepting genial ideas,
however). Let's go on...

I read the comments saying 'be careful' on both front and back. OK,
now are in the way... the area outline is enough for working around it.
Sadly I can't turn off the comment layer since the outline would
disappear too. Also turning off the front text would be hide the
assembly refdes. That's a problem. I could hide the single text entity;
that would work but it's a little inconvenient *especially* if I wanted
to see them later again. 

So, concluding:

- The master reference (the one on silk) has privileged treatment (for
  historical reasons) but it's not too useful once it's in its final
  place (i.e. outside the part). The one on assembly (which is a user
  text) is more useful but doesn't have that treatment. Too bad we can't
  swap them and make the one on assembly the master one :P

- Hiding text selectively when it's in the way *can* be done but is not
  extremely convenient; a script or some mass command (like the 'reset
  sizes') could help, however. Also setting the text display to 'lines'
  greatly reduces the impact of text (when zooming in enough for
  tracking);

- Initially I've had tought of adding a "User Texts" visible checkbox
  for completeness with values and references... it's useless as you can
  see, since it's more or less like using the "Text Front"/"Text Back"
  ones; too coarse;

- The 'final solution' would be to have a text enable on a by-layer
  basis; smell like bloat to me however...

So, unless there are good ideas, I think I'll leave the interface as it
is. Hiding the text with the whole layer content at the moment seems enough good
to work; selective hiding and lines text mode seems to be good
mitigation measures. As a convenience a 'show/hide all text on layer'
command/script could be useful, however that would act on the data
model, *not* on the display.

That would, of course, be my own workflow. Probably someone else has
other ways to do things. A good compromise needs to be found.

Back to coding

-- 
Lorenzo Marcantonio
Logos Srl