[SOLVED] Using Bus Alias across a Hierarchy on Kicad 7

I have a complex schematic with long signal names that connect to a bus over multiple pages of schematics. To simply the amount of text I want to use Bus Alias’ however I cannot get this to work.

To try to understand this I created a simple example with:

  1. A Bus named using a Bus Alias and connecting some component on a single sheet.
  2. The same circuit as 1 but captured over 2 hierarchical pages using a Bus named using a Bus Alias.
  3. The same circuit as 2 but captured over 2 hierarchical pages using a Bus with discrete names.

Example 1 and 3 work but 2 does not. If I am understanding Bus Alias’ correctly 2 and 3 should behave the same but don’t and I don’t understand what I’m doing wrong.

I’m a new user to the forum so cannot post the example database but can make if available if it helps.

I’m a new user to the forum so cannot post the example database but can make if available if it helps.

welcome to the forum. The restrictions are antispam countermeasures. Read the “new member” article on how to promote one user level: New Member Information

As a promoted “basic user” you than can attach your example project (the complete project archive) and we can examine it.

Here is the test file, hoping this helps to solve my issue.

Test.zip (16.0 KB)

first: good example, this makes reproduction easy. If you (at some point in time) maybe report bugs at gitlab: such a example is always appreciated.

Now to your exact schematic: I don’t know why, but the hierarchical sheet pins on the root sheet (inside the sheet-rectangles) for {Test2} are not connected to the bus itself.
Running the ERC shows this problem. Moving the sheet pins a little bit away and redraw the bus connection solves the problem:
test_repaired.zip (16.5 KB)

Not sure that I have an answer to what is going on however, the database I found this on was imported from Altium and had a non-standard grid (2.5 mm versus the default of 2.54).

If I move some stuff around on the repaired database, I end up with the pins being slightly misaligned with the bus so there is some evidence that the bus and the pins are not aligned to the grid despite the grid not changing between add the pins and drawing the bus.

Anyway many thanks, I can not go fix my database.

1 Like

two additional remarks (maybe you have already used that settings/options) which I recommend new colleagues:

  • preferences–>common–>warp mouse to origin of moved object
  • preferences–>schematic editor-_>display–>snap to grid: always
  • be very cautious to release the CTRL-key prior to every mouse-button commit (the CTRL-key temporary disables the grid snapping - so if CTRL is still pressed during placing some item than the symbol/pin/wire/bus ends up offgrid)

You could run the “align elements to grid” command at the end of schematic placement/wiring to ensure good connections of all wires. (this command is available on the RMB-click context menu and works for the currently active selection).
Be aware that this last hint currently don’t works for the sheet-pins (so exactly your use case is not working) if the sheet-pins and the sheet-box are selected at the same time.
So your example delivered the impulse for detecting a bug:)

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.