Application: KiCad
Version: 5.1.7-a382d34a8~88~ubuntu20.04.1, release build
Libraries:
wxWidgets 3.0.4
libcurl/7.68.0 OpenSSL/1.1.1f zlib/1.2.11 brotli/1.0.7 libidn2/2.2.0 libpsl/0.21.0 (+libidn2/2.2.0) libssh/0.9.3/openssl/zlib nghttp2/1.40.0 librtmp/2.3
Platform: Linux 5.4.0-54-generic x86_64, 64 bit, Little endian, wxGTK
Build Info:
wxWidgets: 3.0.4 (wchar_t,wx containers,compatible with 2.8) GTK+ 3.24
Boost: 1.71.0
OpenCASCADE Community Edition: 6.9.1
Curl: 7.68.0
Compiler: GCC 9.3.0 with C++ ABI 1013
Build settings:
USE_WX_GRAPHICS_CONTEXT=OFF
USE_WX_OVERLAY=ON
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_PYTHON3=ON
KICAD_SCRIPTING_WXPYTHON=ON
KICAD_SCRIPTING_WXPYTHON_PHOENIX=ON
KICAD_SCRIPTING_ACTION_MENU=ON
BUILD_GITHUB_PLUGIN=ON
KICAD_USE_OCE=ON
KICAD_USE_OCC=OFF
KICAD_SPICE=ON
In my schematic I used different GND* symbols for different ground nets. Those nets are not connected among them: they come from different connectors are never mix-up.
But if I highlight such a net, all of them (GND, GND1, GND2, etc…) are selected! And in Pcbnew I see they are connected with the same name GND. Why?
Because I used different power symbols, should not they keep separate?
Where do your GND symbols come from?
Did you make them yourself?
The visible text in the GND symbols is just the name of the symbol. The net that the symbol is connected to is derived from the (normally invisible) name of the pin of the symbol that the net is connected to.
You can see this text when by editing it in the Schematic Symbol Editor.
If this does not help, then:
Make a copy of your project.
Delete most of the distracting stuff. Just leave a few of your GND symbols and something to which they are connected (for example a few resistors).
Check that the problem is still present.
Zip the simplified project. make sure that [projectname]-cache.lib is also present.
Yes I was away from my computer just now and remembered. I think I had previously fallen into the problem that paulvdh describes. If you made the symbols, check the pin names in the symbols!
Thanks for the clear answer.
Yes, I did the power symbols by myself but I think I did them well changing the invisible pin name along with the label. Anyway, to be sure in the de-cluttered copy I’m uploading here I used the default supply pin from Kicad libraries. And the problem is still there.
I will be very happy if you can inspect the project. There are only few components and two GND nets: GND and GND1. As said if you highlight any of them all will be selected.
I’m sure I did something wrong but I cannot understand what!
I downloaded your zip file but I am not able to diagnose the problem for at least 2 reasons:
I am running a 5.99 nightly
For GND I think I get my own symbol of that name when I go to edit in symbol editor. For GND1 I get a blank when I go to edit in symbol editor. Probably there is no GND1 in my library.
Anyway this dialog box shows my view in 5.99. You said you checked the pin name but I do think I encountered similar to your complaint due to my not having changed the pin name.
One other comment: I think you set yourself up for confusion by having U2 GND1 pin connected to GND, and U2 GND2 pin connected to GND1. Does not sound so complicated on the surface but working with that would drive me nuts.
On the GND pin of the DRV8872DDARQ1 there is a little black splotch.
This is a label that connects GND to GND1.
If you remove that label, then the schematic is OK.
Such small labels are often a remnant of an eagle to KiCad conversion.
There is also such a label on +24V but that does not cause any problem at the moment, but it’s redundant and probably better to remove it too.
If you also connect “PWR_FLAG” symbols to your input connectors, you remove 4 more ERC errors:
