The cross-probe facility is great… but in a multi-sheet (schematic) design it could be better.
INFO: A user called ‘tom’ asked something similar back in 2018, but he got no responses.
This may have been addressed in v9, but I am mandated to stay with v8 until my current design goes to production (software version changes during a design are all-but forbidden in my workplace).
In a multi-sheet design it is often the case where a signal (eg: SCK) appears on several pages. Clicking a signal on one of the pages highlights the net throughout the design ‘pink’ and highlights the PCB trace, but gives me no hints as to what other pages in the schematic host that signal.
It would be great if the ‘schematic hierarchy’ (design tree) would highlight the pages where said signal appears in the same ‘pink’ colour - especially for designs that have more than 10 pages of schematics… it is a real pain to have to open every page and check if the signal appears on it.
In most cases I can rely on my memory in knowing what pages contain what, but that quickly evaporates moving between projects, and then if I get tasked to rehash an older design to add some functionality (something I’m deep into at the moment) it goes out the window.
Is this a feature in v9, or maybe I should create a ‘wish’ for v10?
How about in V8 ? In the Schematic turn on the Net Navigator and select a net that’s on several pages . . . GND perhaps ? then use the ` key to “Highlight Net”, the Net Navigator will show you which sheets that net is present on. This also cross probes between the Layout and Schematic.
Another function that may be useful in this context is: Schematic Editor / File / Schematic Setup / General / Formatting / Inter-sheet References With this KiCad can add page numbers to labels to the pages where other connections with the same net are.
Yes, of course. Local labels never connect to another sheet, and with hierarchical labels, you have to follow the hierarchy itself. (And signals can get renamed though the hierarchy).
One method I’ve read, (but not used yet myself) is to use local labels for everthing on the sheet. And then, somewhere on the sheet you place a column with global labels with the net names you want to use globally. This works because KiCad connects local labels with global labels on the same page, and thus the label gets promoted to a global label. This looks like a really nice approach. You’ve got a good overview of all global signals that are used on a page, and all the inter-sheet references will also show in that table (and thus not clutter up the rest of the schematic).
