kicad-developers team mailing list archive

[Russell Oliver <roliver8143@xxxxxxxxx>]

Hi all,

Sorry I didn't get to it sooner. Been busy at a new job.

I was going to say that globals will work fine except for the visual
aspect. Though I think just replacing the global net on the pcb with the
net from the schematic with the matching end label ( ignoring any sheet
path)  should work too, since it will be unique anyway if importing from an
eagle schematic.

Kind Regards
Russell


On 17 Feb 2018 10:06, "Maciej Suminski" <maciej.suminski@xxxxxxx> wrote:

Alright, I switched the importer to use global net labels. Perhaps
schematics are not always the prettiest ones, but at least they are
equivalent to the original project.

Cheers,
Orson

On 02/16/2018 02:59 PM, Wayne Stambaugh wrote:
> If using global nets resolves the issue and doesn't cause any other
> issues, it has my vote as well.
>
> On 02/16/2018 08:36 AM, Maciej Sumiński wrote:
>> I vote for switching to global nets. I may handle this, just want to be
>> sure Russell has not started already working on it, so there is no work
>> duplication.
>>
>> Regards,
>> Orson
>>
>> On 02/16/2018 02:17 PM, Wayne Stambaugh wrote:
>>> Gentlemen,
>>>
>>> What is the status of this bug fix?  I know there was some discussion
>>> about this patch.  Do we have path forward on this yet?  I would like to
>>> get this into rc1 if possible.
>>>
>>> Thanks,
>>>
>>> Wayne
>>> On 02/14/2018 08:17 AM, Russell Oliver wrote:
>>>> Please find the attached patch for this issue.
>>>>
>>>> On Tue, Feb 13, 2018 at 2:34 AM Maciej Sumiński <
maciej.suminski@xxxxxxx
>>>> <mailto:maciej.suminski@xxxxxxx>> wrote:
>>>>
>>>>     Hi Russell,
>>>>
>>>>     On 02/11/2018 05:41 AM, Russell Oliver wrote:
>>>>     > Hi All,
>>>>     >
>>>>     > I've discovered the cause of a problem when importing Eagle
>>>>     Projects and
>>>>     > getting the schematic and boards synced.
>>>>     >
>>>>     > Currently when importing an Eagle schematic, labels for nets that
>>>>     are only
>>>>     > found one Eagle sheet are imported as local KiCad labels. This
>>>>     preserves
>>>>     > the visual design of the schematic some what. For eagle
schematics
>>>>     with
>>>>     > more than 1 sheet, where hierarchical sheets are created in
Kicad,
>>>>     global
>>>>     > labels are created to tie the nets together across the sheets the
>>>>     same as
>>>>     > Eagle due to its lack of scopes for net names.
>>>>     >
>>>>     > The problem is that the imported PCB will have net names that are
>>>>     global
>>>>     > e.g "VBUS" while the imported schematic may end up with local
>>>>     netname for
>>>>     > the root sheet e.g "/VBUS". This will cause errors for boards
with
>>>>     zones
>>>>     > and named vias with the original/global netname e.g."VBUS"
>>>>     >
>>>>     > My proposal to fix this is to create another pass in the netlist
>>>>     generation
>>>>     > code that would remove the forward slash '/' for unique local
nets
>>>>     in the
>>>>     > root sheet provided it does not clash with an existing net name.
>>>>
>>>>     Good catch. I would rather not modify the netlist generator code,
but
>>>>     add another pass in the board importer. I suggest the following:
>>>>     - Move netlist generation from kicad/import_project.cpp to
>>>>     SCH_EDIT_FRAME::ImportFile().
>>>>     - Move netlist import from kicad/import_project.cpp to
>>>>     PCB_EDIT_FRAME::ImportFile().
>>>>     - After importing a board and its netlist, go through the list of
zones
>>>>     and try to assign '/' + zone->GetNetname(). If such netlist
exists, then
>>>>     it means the assigned net is a local one and needs renaming. The
only
>>>>     problem here is a potential conflict if there exist both 'netname'
>>>>     (local label) and '/netname' (global label). I guess such case
deserves
>>>>     a huge warning, so the user needs to verify the import result.
>>>>
>>>>     I suppose the last special case should be simply reported by the
ERC
>>>>     even without importing a project, as it creates a connection
between two
>>>>     seemingly not related nets.
>>>>
>>>>     Thoughts?
>>>>
>>>>     Regards,
>>>>     Orson
>>>>
>>>>     > Kind Regards
>>>>     > Russell
>>>>     >
>>>>     >
>>>>     > P.S During debugging this issue, I discovered that a local label
>>>>     and global
>>>>     > label of the same name on the same sheet are connected regardless
>>>>     of any
>>>>     > wires. Which if there is a hierarchical sheet can lead to the
same
>>>>     net for
>>>>     > 2 wire segments on separate sheets connected only to local
labels,
>>>>     if the
>>>>     > identical global label is somewhere else on both sheets. Is this
the
>>>>     > expected behaviour? or just a side effect?
>>>>     >
>>>>
>>>>
>>>
>>
>>
>