2
\$\begingroup\$

enter image description here

enter image description here

I am using Kicad version 4.0.2-stable, which I think is the current version.

I cannot figure out how to get what I presume is the net name GND to “stick” between the schematic editor and the PCB layout editor.

In the first image above, CO2Pad4 is an item I made in the schematic library editor. It has 4 pins, all labeled ‘1’ and is intended to ultimately represent a soldering pad on the PCB. Notice that it is connected to GND by wires.

When the net list is created and imported into the PCB layout editor, Pcbnew, Kicad gives it a net name of Net-(CO2Pad4-Pad1) rather than GND. This prevents the rat’s nest from showing a connection between CO2Pad4 to GND, and thus Kicad will prevent a trace being drawn from the CO2Pad4 to ground.

I have found that in PCB layout editor, Pcbnew, I can change the net name for CO2Pad4 from Net-(CO2Pad4-Pad1) to GND and then the rat’s nest will show a connection.

The problem is that when I make a change to the schematic, Kicad reverses this change. On a more complicated circuit, I am afraid that I will miss the reversion.

I have tried both local and global labels applied to the wire connecting to CO2Pad4 to no avail. I thought I had solved it when I applied a global label to a pin on CO2Pad4 (again, all the pins are number '1') and a global label to the wire connecting to the GND symbol on the right side of the first figure. That worked, until…

I have another, grounded connection pad, CO2Pad2, elsewhere in the circuit. When I applied the global label GND to one of its pins, Pcbnew applied the net name GND to the second pad, but reverted to Net-(CO2Pad4-Pad1) for the first pad!

Since the local label symbol in the schematic editor indicates that it is a “net name - local label”, I am puzzled as to why this is so hard.

Thanks for any suggestions.

\$\endgroup\$
0
\$\begingroup\$

You need to use the "Wire" name feature to keep a name to stick on a net, so name the schematic wire GND. 4.x seems to not be a nice for pin names propagating.

\$\endgroup\$
  • \$\begingroup\$ If you are referring to a "net name - local label", the black 'A' with a green underline, I tried that and it did not work. If there is another "wire name" feature, could you point it out? \$\endgroup\$ – user34299 Aug 4 '16 at 20:13
  • \$\begingroup\$ that should work unless there's a conflict. do you have an old GND symbol and a newer one (from the .pretty library). for some reason there's a bug on global labels. I've had a helluva time porting my schematic due to that. so where's the other GND and why can they not be connected, is the question \$\endgroup\$ – b degnan Aug 4 '16 at 20:32
  • \$\begingroup\$ I do have multiple instances of the GND symbol, though all are from the same .pretty library. Just to confirm, Kicad should see the GND connected symbol as a net name, correct? \$\endgroup\$ – user34299 Aug 4 '16 at 22:49
  • \$\begingroup\$ yeah, it should. Do you have another GND label somewhere? BTW, I just confirmed that the "label" takes precedence over global names. \$\endgroup\$ – b degnan Aug 5 '16 at 0:38
0
\$\begingroup\$

In another discussion it was suggested that my connecting only one of the four pins on the connection pad to GND had "confused" Kicad, even though all the pins were numbered '1'. It was suggested that the pins be numbered one through four and then all four connected, via wires, to the GND power point. Before I did that I simply connected all four of the pins together and via a wire to the GND power point, all still numbered '1', and the problem was solved!

I was thinking that since all the pins were numbered '1' that Kicad would have connected them automatically, but that is apparently not the case.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.