kicad-developers team mailing list archive

[Maciej Suminski <maciej.suminski@xxxxxxx>]

If I recall correctly, you are allowed to name an alias using <name>
format, so there is nothing preventing you from doing so. I would rather
not impose such constraint on aliases, but I am interested in other
opinions.

Regards,
Orson

On 12/14/2017 01:09 PM, kristoffer Ödmark wrote:
> Maybe we could adapt from c++ here? having the notation <ALIAS> instead
> of {ALIAS}, the same way c++ uses templates.
> 
> one could do MEMORY{<RAM> D[15..0]}. And get MEMORY.OE MEMORY.WE and
> MEMORY D15 etc. Just to be more clear that it is an alias and not a
> net-name.
> 
> - Kristoffer
> 
> 
> On 2017-12-14 12:43, Clemens Koller wrote:
>> Hello, Jon!
>>
>> Thank you for your work! I just watched your video and want to give
>> you some feedback:
>>
>> I would prefer not to use the term "Bus Vector". A bus is simply a
>> list (or a collection) of arbitrarily named nets. A bus group would be
>> - in my understanding - a group of (different) busses.
>>
>> I like your syntax to represent the list (or collection) {} as well as
>> an array of nets [].
>> You first had a bus containing arbitrary nets: MEMORY{A{7..0] D[15..0]
>> OE WE} and you refer to single nets as i.e. MEMORY.A3 or MEMORY.OE -
>> fine.
>>
>> But when you add aliases I run into troubles to keep things
>> separate/clear:
>> {RAM} appears to me as an unnamed bus containing the net RAM. WTF is
>> that?
>>
>> MEMORY{RAM} appears as a bus named MEMORY containing the single net RAM.
>> I would expect to access that net via MEMORY.RAM - Oops.
>>
>> I am definitely irritated by a net MEMORY.OE pulled out of an bus
>> named MEMORY{RAM}. 8-(
>> It's impossible to distinguish bus aliases from nets of a bus.
>>
>> Idea: It might be nice to virtually allow folding/unfolding of the net
>> collection contained in a bus, i.e. by showing MEMORY{*} or MEMORY{..}
>> or MEMORY{+}, whereas the '*' or '..' or '+' is shown in a different
>> colour. If that's still to long, I would not mind renaming the bus to
>> MEM{..} or even M{..}.
>> A simple mouseover M{..} could pop-up to show all nets and arrays the
>> bus contains.
>>
>> Side note: For big designs, table-based design entry (as well as
>> design entry by importing tons of generated connections) seems to get
>> more and more important. It might be wise to consider how busses (and
>> collections of <something>) are represented there as well.
>>
>> Just my five cents,
>>
>> Clemens
>>
>> On 2017-12-14 05:15, Jon Evans wrote:
>>> Hi all,
>>>
>>> As some of you know, I've been working on some new features for
>>> Eeschema that expand the capabilities of buses.
>>> These features are not yet complete, but I wanted to share my
>>> progress to get early feedback.
>>>
>>> Since there are a number of things, I have made a ~4 minute demo
>>> video, in which I walk through them and discuss:
>>>
>>> https://youtu.be/z6x0xiKgDIc
>>>
>>> In case you don't want to watch the video, here are the new features:
>>>
>>>    * The existing style of bus is now referred to as a Bus Vector
>>> (for example: "A[7..0]")
>>>    * New concept: Bus Groups, for adding arbitrary nets to a bus
>>>        o Defined in a list, separated by spaces, enclosed in curly
>>> braces. For example: "{DP DM}"
>>>        o Can contain bus vectors as well as plain nets, for example
>>> "{A[7..0] D[7..0] OE WE}"
>>>        o Can have an optional name in front, like "MEMORY{A[7..0]
>>> D[7..0]}"
>>>        o If you add a name, the resulting nets will have the name
>>> prefixed on the front, like "MEMORY.A7"
>>>    * New concept: Bus Aliases
>>>        o You can use aliases to define shortcuts for bus groups.
>>>        o For example, you could create an alias called "USB" that
>>> refers to the nets "DP" and "DM"
>>>        o Then, you can define a bus group as "{USB}" which will
>>> contain both of those nets.
>>>        o You can also add a label, like "USB1{USB}" which will result
>>> in nets "USB1.DP" and "USB1.DM <http://USB1.DM>"
>>>        o Bus Aliases are editable through a new dialog, and saved
>>> with the schematic file.
>>>    * New tool: Bus Unfolding
>>>        o Right click on a bus, and you can easily break out any of
>>> its members into a bus entry, label, and wire.
>>>        o You place the label (and set the bus entry orientation) with
>>> the first click, and then can continue wiring.
>>>
>>> In order to support this work, I am also working on a new
>>> connectivity algorithm for Eeschema.
>>> This algorithm stores the resulting connectivity information with the
>>> graphical objects on the schematic, meaning that it's quite easy to
>>> look up what net any particular object is part of.  The new algorithm
>>> is also significantly (i.e. an order of magnitude) faster at
>>> generating connectivity than the current netlisting algorithm in my
>>> testing so far.  It will support partial updates of the connectivity
>>> when editing the schematic, so the net information will always be in
>>> sync when adding/removing/editing items in the schematic.
>>>
>>> The combination of a faster algorithm and caching of the connectivity
>>> results in dramatic speedups when working with large designs.
>>> For example, Chris' motherboard project (which is a great benchmark,
>>> by the way!) takes several seconds to highlight nets in the current
>>> master branch, and with my changes, you can highlight any net
>>> instantaneously.
>>>
>>> Although it is not yet far enough along to demonstrate this, I plan
>>> to use this new connectivity algorithm to generate netlists for
>>> export, and replace the existing algorithm entirely.
>>>
>>> You can check out the code in my branch here, but be warned that it
>>> is not yet complete, so I am not yet proposing that anyone do
>>> exhaustive testing of it and report bugs (because I already know
>>> about many of the bugs you will find :-)
>>>
>>> https://github.com/craftyjon/kicad/tree/bus_upgrades
>>>
>>> Thanks,
>>> Jon
>>>
>>>
>>> _______________________________________________
>>> 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
>>>
>> _______________________________________________
>> 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
> 
> 
> _______________________________________________
> 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