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 : [email protected] >>>>> Unsubscribe : https://launchpad.net/~kicad-developers >>>>> More help : https://help.launchpad.net/ListHelp >>> >> _______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
