I am trying to make a sheet entry to use ports to connect devices in different sheets as explained in this image:

enter image description here

But I am getting an error from Altium saying:

Sheet Entry RB[0...7]
Warning: Nets whit multiple names
Error: Nets whit possible connection problems

Of course, nets are not being connected on the PCB. It is my sheet entry:

enter image description here

As you can see there is a red line below RB[0...7]. I want to connect a bus between the two sheets. If I put a simple pin instead of a bus I get the same error so I suppose the problem is in the sheet entry and not on the other sheets. My project looks like:

enter image description here

Thank you for your help :)


Esquema PIC.SchDoc: enter image description here

Entrada Analizador Logico.SchDoc:

enter image description here

Settings: enter image description here

PCB enter image description here

I can't see any differences between your examples and my sheets

SOLUTION @Fake Name answer was ok, you have to name ports and net labels as RB[..] not RB[...] (2 points instead on three) and you have no put a Port in each bus AND a net label also whit the same name in order to connect them.

  • \$\begingroup\$ Regarding your edit: The only difference I see between your example and Fake Name's example is that you use 3 dots for the bus' net label. Try using RB[0..7] instead of RB[0...7]. That's the way it's recommended in the Altium manuals too. \$\endgroup\$
    – m.Alin
    Commented Jul 25, 2012 at 11:43
  • 1
    \$\begingroup\$ Ok, problem solved, I didn't put net label on each bus, you have to put Port AND Net Label in order to connect them. Also I have changed [...] to [..] as you recommend me thank you :) \$\endgroup\$
    – Andres
    Commented Jul 25, 2012 at 11:52
  • \$\begingroup\$ @Andres - I mention the buses have to be named too. Look at the end of my answer: For what it's worth, I am fairly sure you have to both name the buses with net-labels on each child-sheet, and name the ports. \$\endgroup\$ Commented Jul 26, 2012 at 5:24

1 Answer 1


Can you post your sub-sheets?

From looking at what you have posted, I think you may have a typo in the entry: RB[0..7]. You typically get the red line below the entry when it is not correctly tied to a port on the child-sheet.

Right-click on the sheet symbol, and select "Sheet Symbol Actions" -> "Synchronize Sheet Entries and Ports"

enter image description here enter image description here enter image description here


I created a simple, minimal test schematic to do what you are doing:

Top Sheet: enter image description here
Sheet 1:
enter image description here
Sheet 2:
enter image description here

Project Hierarchy:
enter image description here

And it properly connected the nets across the different schematics:

enter image description here

For what it's worth, I am fairly sure you have to both name the buses with net-labels on each child-sheet, and name the ports.
Also, the bus name and wire names have to have the same prefix:
For example, a set of wires HERP0 HERP1 HERP2 HERP3 HERP4 has to be in a bus named HERP[0..4]. It may also have to be zero-indexed (i.e. start at 0, rather then 1), but I'm not totally positive on that.

Also, I do indeed get the "Net NetName has multiple names" warning, but it's just that, a warning. You can turn the warning off, or just ignore it. I tend to leave it on, and before I have a board produces, go through all the warnings and make sure that I intend for whatever they refer to to be that way.

  • \$\begingroup\$ Fake Name, I have edited my questions whit my sub-sheets. In "Synchronize Sheet Entries and Ports" options Altium says "All sheet symbols are matched" on the sheet entry where I have RB[0...7] and where I have A[0...7] port I have matched it but keep getting the same error. I saw one of my port in sheet entry was bi-directional and the other not, I changed both to bi-directional and the error dissapeared but they are not being connected on PCB. \$\endgroup\$
    – Andres
    Commented Jul 25, 2012 at 11:40

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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