Hello
I want to change fron Eagle to Kicad. Some projects coverted fine. Now I have a project
where 2 GND nets are used for electrical isolation. Nets are named GND and GND2.
When I import this project, there is only one GND net in schematic. In PCB the nets
are labeled GND and GND2. The DRC shows hundreds of errors, as GND2 don’t exist in schecmatic.
How can I fix this problem, to not reroute all GND?
There is not much to write here without having a look at your files.
If a net is shorted to some other net (for example GND and GND2) in even a single location, then KiCad merges those nets into a single net. Usually it does generate an ERC message for this, but if you have hundredths of them, then it’s easy to miss.
Also, do note the difference between ERC Electrical rule check, which is on the schematic, and DRC Design rule check, which is on the PCB.
Thanks for your answer! The previous eagle design was ok and had no connection.
Attached find the eagle files!
646-RKP_VidV1a.brd (341.1 KB)
646-RKP_VidV1a.sch (1.8 MB)
KiCad does give this warning (With default settings):
And clicking on the line with “Label ‘GND2’” shows the location:
The reason the nets are merged is because KiCad imports the triangular symbols as a power symbol with a GND name for the pin. KiCad also imports (or generates) the GND2 label. So that results in two different names, and thus KiCad merges the nets together.
To fix it, just delete the GND symbol from that single net, or replace it with one of KiCad’s native other GND symbols, such as GND2.
I have done some eagle to KiCad conversions for fun and did the initial port for the Roscoe-M68K project, and in general I replace (most of) the imported symbols with native KiCad symbols. KiCad has quite nice tools for symbol replacement, and using native KiCad symbols just look better to me.
Hello
Thanks a lot ! Problem solved! There have been also some other problems with supply voltage connections.
Changing the symbol solved it!
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
