kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxx>]

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
>