Global and local net connections different in v9 than v8

Schematic
1

In some of my schematics, I have a long list of test points off to one corner of the schematic. All the nets are wired up nicely, but the test points were added later (due to a change in factory) and they ended up all in one place instead of sprinkled about the schematic on their respective nets.

The designs are also hierarchical using only global nets for all intrasheet connections.

Under v8, the global net labels and the local labels for the test points merged into a single net. This schematic design was no problem. But after updating to v9, I get lots of ERC issues. Something in Eeschema has changed.

I have found 2 issues:

  1. In v8, the box on a local label could be anywhere on the wire. In v9, the box for the label must lay on top of the box for the end of the wire.
  2. In v8, global ports into a hierarchical block carry a global net name and a simple net label inside the same hierarchical block with the same net name with be merged into the same net. In v9, they are treated as different nets and trigger an ERC warning about global and local nets with the same name.

To help explain this, I’ve created a simple test case with my v8-style schematic that shows the same issues I described above. See the two ERC errors created by the test point on the VIN net in ‘sheet1’.
v8_global_local_nets.zip (31.4 KB)

I can fix #1 above relatively quickly and easily by moving my local labels around. But #2 is more difficult and time-consuming, with the only solution I can find being to move the test points onto the wire of the global net that I want them to attach to. As I have dozens of test points, I’d like to find a way around this that doesn’t consume my time manually updating the schematic. Are there any other solutions to either of the changes I observe in v9 vs. v8?

I have not seen other posts about this, but forgive me if I missed them.

2

First: To have a comparison between v8 ↔ v9 you have to attach your example project as v8 version. With your provided example (v9) I can’t compare with the previous version.

But looking at the provided project with kicad v9 all looks good.
There are just additional /modified checks for the ERC, which trigger new ERC warnings.

  • your problem #1: warning unconnected wire endpoint. This is just a warning, and it’s correct: the wire endpoint at coordinate 1.8/6.6 (inch) is dangling unconnected. Nothing bad about that, but the corresponding ERC check finds this. If you work more often with this type of drawings and like it → then turn off this specific ERC check
  • your problem #2: warning “local and global label have same name” is just a warning. The nets are still merged together. You may check this if you enable the net navigator panel (View–>panels–>net navigator) and subsequently highlight (not select) the net. For your workflow it’s probably useful to also turn off this check.

It’s your task as a designer to decide if ERC warnings are important for you and which warnings provoke too much noise (false positives) on your specific workflow.

3

For info, these were the announcements for the new ERC checks:

1 Like