kicad-developers team mailing list archive

[Chris Pavlina <pavlina.chris@xxxxxxxxx>]

I'm in favor of power connects as labels because, well, that's what they
are! Remember that power components and global labels behave
identically. IMO keeping this consistency is very, very good from a user
interface perspective - components in general don't make connections to
remote places, that's what labels are _for_. The idea of a special type
of component that behaves like a label really does not sit right with
me.

It's also a quicker, more direct way to place a power port; there's no
need for the separate edit step.

Editing the value is a compromise I wouldn't be too upset about
accepting, though I still think my way is better ;)


On Mon, Aug 01, 2016 at 01:42:05PM -0400, Wayne Stambaugh wrote:
> How is this different or better than being able to edit a power
> component value?  I know we cannot do this right now but I see no reason
> that it couldn't be done once the new file format is in place and power
> components are defined by component type rather than naming semantics.
> 
> On 7/31/2016 5:09 PM, Chris Pavlina wrote:
> > Power labels replace power components. Here are a couple screenshots
> > from my feature branch that I dug up - still haven't actually got it
> > building again, it had a few issues, but the screenshots should explain.
> > Bear in mind they're all at different levels of development, so I don't
> > necessarily mean things should be *exactly* like this.
> > 
> > https://misc.c4757p.com/power.png
> > https://misc.c4757p.com/powereditor.png
> > 
> > I implemented them as a subclass of global labels, with a modfied draw
> > method that would render a library part instead of a text label. I then
> > embedded a library of standard power symbol styles so the user could
> > simply select one, and added a property to the labels to record their
> > style. Future plans included the ability to use user-supplied styles,
> > edited by the library editor.
> > 
> > It's not immediately obvious from the screenshots, but the UI had
> > heuristics to pick a sensible style based on the net name you typed, so
> > power labels could be placed very quickly by pressing the hotkey (I just
> > repurposed P), typing the power net name and hitting enter.
> > 
> > Allowing user-supplied styles would allow backwards compatibility with
> > old schematics: old-style power components in those schematics could be
> > simply converted to power labels using that component as the style; no
> > visual or logical difference would occur.
> > 
> > On Sun, Jul 31, 2016 at 04:59:53PM -0400, Wayne Stambaugh wrote:
> >> On 7/31/2016 4:45 PM, Wayne Stambaugh wrote:
> >>> On 7/31/2016 3:59 PM, Chris Pavlina wrote:
> >>>> On Sun, Jul 31, 2016 at 03:25:11PM -0400, Wayne Stambaugh wrote:
> >>>>> On 7/30/2016 9:22 PM, Chris Pavlina wrote:
> >>>>>> Hi,
> >>>>>>
> >>>>>> I was reading through the new sch/lib format documents posted back in
> >>>>>> February: https://lists.launchpad.net/kicad-developers/msg23302.html
> >>>>>>
> >>>>>> Since work is underway to facilitate adding this now, I figured it was a
> >>>>>> decent time to bring up a few concerns and suggestions I have. Bear in
> >>>>>> mind I'm working off a pretty old version of the document here - if it's
> >>>>>> been updated and some of this has changed, feel free to point me to a
> >>>>>> more recent version; I couldn't find one.
> >>>>>
> >>>>> I don't believe I've changed it since the last time I published it on
> >>>>> the mailing list.
> >>>>>
> >>>>>>
> >>>>>> - I think we should work to reduce redundancies in the format. They just
> >>>>>>   confuse things and introduce parsing complexities (what happens when
> >>>>>>   A implies B, both are written to the file, and they don't agree with
> >>>>>>   each other?). Examples:
> >>>>>>
> >>>>>>   - Why both 'polyline' and 'line'? Surely eeschema isn't going to get
> >>>>>>     tired of writing 'poly' and decide to start abbreviating it? Can't
> >>>>>>     we remove one?
> >>>>>
> >>>>> Agreed. 'lines' could be one or more lines that may or may not form a
> >>>>> polygon.
> >>>>>
> >>>>>>
> >>>>>>   - Arcs have redundant information, we only need either (radius, start
> >>>>>>     angle, end angle, center), or (start point, end point, center). I
> >>>>>>     suggest sticking to the former and dropping the start/end points.
> >>>>>
> >>>>> We currently save all of this information in the for an arc.  I'm not
> >>>>> sure why.  I'm fine with this proposal.  One advantage to using the end
> >>>>> points rather than the angles is round errors to ensure completely
> >>>>> enclosed drawings but I don't know if that is an issue or not.
> >>>>
> >>>> Very good point about the start/end points. eeschema doesn't currently
> >>>> support that - it can't fill enclosed regions that are enclosed by
> >>>> multiple graphical objects - but this would ensure it could in the
> >>>> future with minimal changes. Okay - I'm for using start/end instead of
> >>>> angles, then. I'd still like to get rid of the redundant info, though.
> >>>>
> >>>>>
> >>>>>>
> >>>>>> - Can we consider adding power ports as a type of label rather than
> >>>>>>   component, so we don't have to maintain libraries of every possible
> >>>>>>   rail name anymore? I'd happily contribute to the implementation - I
> >>>>>>   have an old feature branch where I did exactly that, it worked really
> >>>>>>   well :)
> >>>>>
> >>>>> I thought that was in there already.  Maybe I missed it.  There will be
> >>>>> a symbol type token.  We have to support normal, power, virtual (show up
> >>>>> in BOM but not netlist, could have a better name not-in-netlist?), and
> >>>>> not-in-bom? (for net ties at a minimum, maybe net-tie would be a better
> >>>>> name but it could be used for other not in BOM objects that we have yet
> >>>>> thought of).
> >>>>
> >>>> Hm, I don't see it if it's there. I'm not entirely sure what I'm
> >>>> imagining you describing, here. Anyway, I think I'll drop this briefly,
> >>>> and then later resurrect that feature branch I had and start some
> >>>> discussion. I had quite a bit there, including UI work, that was quite
> >>>> slick IMO. :)
> >>
> >> Sorry.  I misread your suggestion although we do need additional symbol
> >> types.  I'm not sure how power labels versus power components would
> >> work.  I would need more information on how they would behave.  Do they
> >> replace power symbols or complement them?
> >>
> >>>>
> >>>>>
> >>>>>>
> >>>>>> - There's a vague comment that fonts aren't supported yet but may be in
> >>>>>>   the future. We should specify *now* how upcoming pre-font versions of
> >>>>>>   kicad should handle future files that have been saved using fonts, and
> >>>>>>   make sure they actually can.
> >>>>>
> >>>>> Yep, that code will need to be tested.  The EDA_FONT object already can
> >>>>> format itself to s-expr it just hasn't been tested yet.  Now that
> >>>>> freetype is a dependency, I'm hoping we can do some more interesting
> >>>>> things with fonts in PCBs.  In schematics, custom fonts are less
> >>>>> problematic other than the age old issue of font availability.
> >>>>
> >>>> Nice. And while I see where you're coming from (and agree) about custom
> >>>> fonts being less useful in schematics, I think if we did implement that,
> >>>> it would prove very popular. One BIG benefit would be the ability to
> >>>> properly support arbitrary Unicode characters.
> >>>>
> >>>>>
> >>>>>>
> >>>>>> - It looks like the new format may allow an arbitrary number of
> >>>>>>   "alternates", not just the one "De Morgan equivalent" that we allow
> >>>>>>   now. Is this true? I'd love that.
> >>>>>
> >>>>> Yes, don't see any reason that there is only a single alternate body
> >>>>> style.  It will require changes to the component editor.
> >>>>
> >>>> Yup. I'd like to see the component editor changed anyway, ideally by
> >>>> nuking from orbit >:D
> >>>
> >>> Michele is working on a tree view paradigm for the component editor so
> >>> that work is already underway.  I think we see some significant
> >>> improvements in that area soon.  I need to get the file format stuff
> >>> done first.  The tools to edit the new features can happen later.
> >>>
> >>>>
> >>>>>
> >>>>>>
> >>>>>> - Can we ditch 'keywords'? It's not useful anymore, the new component
> >>>>>>   search doesn't use it and does a fine job of sifting through tokens in
> >>>>>>   descriptions.
> >>>>>
> >>>>> We may not want to throw them out.  They could be useful for third party
> >>>>> tools.  I'm thinking tags here which is probably a better token than
> >>>>> keywords.  I'm not dismissing this idea but I have a feeling that they
> >>>>> could prove useful.
> >>>>
> >>>> Fair enough.
> >>>>
> >>>>>
> >>>>>>
> >>>>>> - "Are there any other per net hints besides net classes?" - we should
> >>>>>>   allow them! They're just hints - allow the format to have arbitrary
> >>>>>>   ones that will just be ignored by a pcbnew that doesn't understand
> >>>>>>   them.
> >>>>>
> >>>>> They are called properties in the board file format and they can be
> >>>>> define in any object.  I plan on using that same paradigm in the new
> >>>>> schematic file format.  Properties are for third party tools which kicad
> >>>>> knows nor cares anything about.  AFAIK there is no limit to their use or
> >>>>> definition and they are simple key/value pairs.
> >>>>>
> >>>>>>
> >>>>>> - Can we add controllable line _color_ as well as style? And also for
> >>>>>>   wires? (people making wiring diagrams will like that.)
> >>>>>
> >>>>> I don't see any reason not to add an optional color expression to all
> >>>>> objects where it makes sense.  Of course the code will need to be added
> >>>>> to the objects (EDA_ITEM?) themselves and fall back to the defaults when
> >>>>> no color is defined.
> >>>>>
> >>>>>>
> >>>>>> - BUG: bus_entry is missing an angle specifier - it's possible to
> >>>>>>   rotate/flip them.
> >>>>>
> >>>>> Good catch.
> >>>>>
> >>>>>>
> >>>>>
> >>>>> A few more that didn't make it into the latest spec but I'm planning on
> >>>>> implementing:
> >>>>>
> >>>>> * Embedded components with an option to link.  Initially linking will
> >>>>> only support internal linking but eventually it will grow to support
> >>>>> other external linking such as file, ftp, http, etc.  The link format
> >>>>> will be a uri.  For internally linked components the format will look
> >>>>> something like sch:\\SCH_NAME\COMPONENT_NAME.
> >>>>
> >>>> I'm not sure how I feel about this. I like the idea, but I'm not sure
> >>>> how this would work from the user's perspective. I can't really think of
> >>>> something that wouldn't be a big pain.
> >>>
> >>> Are you talking about the embedding or the linking?  If it's the
> >>> linking, the default would be embedded.  The linking would be optional.
> >>> Linking to external object is a valid method.  It's what we do now only
> >>> it's limited to the currently defined symbol libraries.  There are users
> >>> (few but they exist) who like to have their schematics (and footprints
> >>> in boards for that matter) track changes they make to symbols.  The
> >>> beauty of the making links optional is the responsibility for breaking a
> >>> design falls on the user not on KiCad.  Most users wont use links but if
> >>> we don't allow them, you can be rest assured someone will complain.  I'm
> >>> willing to forego the linking (it would make life easier) if no one
> >>> finds it useful.  Do other EDA packages allow linking?
> >>>
> >>>>
> >>>>>
> >>>>> * I am considering forgoing the unitless idea at least in the first
> >>>>> pass.  As much as I like the idea, the task of implementing it would be
> >>>>> monumental and I just don't want to change that much of the Eeschema
> >>>>> internals in one shot.  I'm already having to make way more changes than
> >>>>> I'm comfortable with to support the new I/O plugin.
> >>>>
> >>>> YES. I'm 100% for dropping unitless. It's already caused some headaches
> >>>> with people wanting to conform to standards that require things in
> >>>> certain units. What I would like to see, though, is eeschema no longer
> >>>> depending on specifically imperial units - I get that the libraries
> >>>> would be designed around one unit system or the other, but I'd like the
> >>>> option to make a custom set of libraries in metric, for instance.
> >>>
> >>> I'm not 100% sure I want to tackle user defined units in files.  I see
> >>> too much opportunity for floating point rounding issues between files
> >>> defined with different units.  I understand the appeal but my gut tells
> >>> me it's implementation is fraught with peril.  I am more in favor of an
> >>> internal base unit and convert to user units on the fly like Pcbnew.  It
> >>> may be something we can discuss in version 2 but we already a long list
> >>> of new features to implement.
> >>>
> >>>>
> >>>>>
> >>>>>
> >>>>> _______________________________________________
> >>>>> Mailing list: https://launchpad.net/~kicad-developers
> >>>>> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> >>>>> Unsubscribe : https://launchpad.net/~kicad-developers
> >>>>> More help   : https://help.launchpad.net/ListHelp
> >>>
> >>