← Back to team overview

kicad-developers team mailing list archive

Re: [RFC] Remove bus joining behavior from KiCad after 5.0 release

 

Let's not forget the pending wishlist item Bug #1419146 <https://bugs.launchpad.net/kicad/+bug/1419146> to support buses of named members.

You shouldn't have to remember that I2C_DATA is better known as I2C_0 and I2C_CLOCK is I2C_1. Or was I2C_CLOCK = I2C_0 and I2C_DATA = I2C_1?

Extending this idea so a bus can contain another bus makes sense. Let's take an LCD display. In addition to the 4 or 8 data lines, there are several control lines that should be part of the bus. I want an LCD bus that contains LCD_E, LCD_RS, and LCD_RW as well as LCD_D[0..7]. And while I'm fantasizing, I want the bus name to be "LCD"; I do NOT want it named "LCD_E,LCD_RS,LCD_RW,LCD_D[0..7]" the way it is in Eagle.

-Reece

On 04/15/18 22:39, Seth Hillbrand wrote:
Hi Jon-

The major issue I think we would need to address is migration.  I don't think that only an ERC warning is sufficient in this case.  Users will rightfully expect that their old schematics will generate valid netlists when opened in a newer KiCad.

One option here would be to translate the implicit net connections into explicit ones when bus junctions are encountered.  Unfortunately, I think that this feature is lightly used, so we might not get much user feedback until they encounter problems and then the problems will be very bad

An alternative might be to increase the functionality of the bus junction. Spitballing here but we might add a "mapping table" dialog that allowed the user to specify the winning name and mapping order.  That should address your points 2-3 although point 4 might be the issue.  I think we could have a default mapping that follows the expected convention but allow users to change it by double-clicking on the junction and editing the mapping table.  Then previous users could keep their functionality while still allowing the arbitrary member arrays you are building.

Thoughts?
-S


2018-04-15 16:40 GMT-07:00 Jon Evans <jon@xxxxxxxxxxxxx <mailto:jon@xxxxxxxxxxxxx>>:

    Hi all,

    I am proposing to remove some behavior from KiCad as part of my
    bus connections changes.  I know we generally don't remove
    features in new releases without good reason, but I think this is
    an exceptional case.

    The user manual describes a way in which you can connect multiple
    different buses together with junctions.  If you aren't already
    familiar with this behavior, please check out the manual:
    http://docs.kicad-pcb.org/stable/en/eeschema.html#wires-buses-labels-power-ports
    <http://docs.kicad-pcb.org/stable/en/eeschema.html#wires-buses-labels-power-ports>

    The section in question is called "Global connections between
    buses" and comes with the following image and describes how these
    bus wires with different labels are connected together:

    Allowing this kind of behavior is problematic for a number of reasons:

    1. It means that net wires and bus wires behave differently, since
    net wires can't have more than one label.  This is potentially
    confusing for users.

    2. It means that junctions need a lot of special logic in order to
    resolve which "branch" of a bus is called what name (for example,
    what if one of those three branches in the above image didn't have
    a label? What would its nets be called?)

    3. Maybe most importantly, it breaks the label->netlist paradigm,
    since an electrical net will only have one label in the eventual
    netlist, and there is no way to determine which label should "win"

    4. I don't think there's a way to map this behavior onto the new
    bus system I have built that allows arbitrary bus members (instead
    of just a sequential vector) in a way that would make any sense to
    the user.

    My proposed changes in this area are as follows:

    1. Remove this section from the user manual.

    2. In my new connectivity algorithm, treat all connected bus wire
    segments as being part of the same bus (meaning they all will have
    the same "name")

    3. Add an ERC warning about having more than one label attached to
    a bus (the warning would appear in the case of the example picture
    above)

    4. Add a note to the user manual stating that this warning is new
    for 6.0

    The only downside that I can see in this approach is that any
    users who relied on this feature will suddenly get new ERC
    warnings.  But I think that this is an "anti-feature" in that it
    creates confusion instead of adding value, so we should nudge
    anyone who uses it towards a different approach.

    Anyone see any issues with this plan?

    Thanks,
    -Jon

    _______________________________________________
    Mailing list: https://launchpad.net/~kicad-developers
    <https://launchpad.net/%7Ekicad-developers>
    Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
    <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
    Unsubscribe : https://launchpad.net/~kicad-developers
    <https://launchpad.net/%7Ekicad-developers>
    More help   : https://help.launchpad.net/ListHelp
    <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



Follow ups

References