kicad-developers team mailing list archive

[Maciej Sumiński <maciej.suminski@xxxxxxx>]

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?
>

Attachment: signature.asc
Description: OpenPGP digital signature