1
\$\begingroup\$

I am struggling to find a way to get the compiler in Altium to see a Sheet Entry/Port (tried with both) and a net label on the same sheet to link.

This redacted schematic page shows what I have (this all on one page, with the relays themselves and drivers etc. all on a second page):

Schematic with Off sheet connector and unconnected net label

But when compiled, it complains of two nets with the same name (that's sort of the point...)

Compiler error

And in the PCB, it wont link the two together:

Board with no connectivity

I have found a workaround and that is to add the net label next to the off-sheet connector/port:

enter image description here

The problem with this however is that there's not always space to have each net name written out twice.. For the relay1 and relay2 signals used in this example, the off-sheet connector sits right next to the title block for the schematic sheet. It can't move any further to the right to accommodate what would be useless duplicate text.

Anyone know of any settings to allow net labels and off-sheet connectors/ports to connect on the same sheet?

EDIT: I've though of another workaround, though it's much more of a bodge - a tiny Net label that's basically invisible:

Bodge...

\$\endgroup\$
3
  • \$\begingroup\$ Are you using a hierarchal or flat project structure? \$\endgroup\$
    – Araho
    Commented Dec 5, 2019 at 12:39
  • \$\begingroup\$ flat, but in reality it does't make any difference as Ports behave the same as off-sheet connectors*. There is an argument for using global net names, but as a house style type thing, we'r rather not * with respect to connections on the same page \$\endgroup\$
    – Chuck990
    Commented Dec 5, 2019 at 13:24
  • \$\begingroup\$ I've found a post in the Altium forum that has a similar issue, with the fix being to add a net label next to the port... forum.live.altium.com/#posts/217359/624710 Really don't want that to be the answer but looks like it will be \$\endgroup\$
    – Chuck990
    Commented Dec 5, 2019 at 14:03

2 Answers 2

Reset to default
1
\$\begingroup\$

I believe that's what the "Allow Sheet Entries to Name Nets" and "Allow Ports to Name Nets" checkboxes in the Project Options window are used for. Go to Project -> Project Options -> Options tab and check these boxes within the "Netlist Options" panel:

enter image description here

I believe this will do what you want it to do.

Note that the Off-Sheet Connectors are really only there for backwards-compatibility with legacy software projects. Newer projects should probably use Ports instead of Off-Sheet Entires.

\$\endgroup\$
2
  • \$\begingroup\$ If I allow Ports or Off-Sheet Connectors to name nets, I still get an error in the compiler stating that I have duplicate NET names. In the PCB, although they share the same name, they don't want to connect to each other (when in routing mode, if I try to connect the two it actively prevents connection, as it would to any other net) \$\endgroup\$
    – Chuck990
    Commented Dec 5, 2019 at 13:47
  • \$\begingroup\$ I don't think the ports/off-sheet connectors will produce errors indicating duplicate net names if you set your project to hierarchical (recommended). This is how I design all of my schematics. You simply need a top-level sheet showing how the other sheets are connected \$\endgroup\$
    – DerStrom8
    Commented Dec 5, 2019 at 16:28
0
\$\begingroup\$

According to Altium documentation, Off Sheet-connectors are only useful for connecting between multiple child-sheets of a given parent page (https://www.altium.com/documentation/altium-designer/sch-obj-crosssheetconnectoroff-sheet-connector-ad). To me, that reads like it only works with hierarchical projects.

Also, you can't connect a Net Label with an Off Sheet-connector, only another Off Sheet-connector.

If you are using a flat project structure, you should use either Net Labels or Ports. If you are using a hierarchical structure, you need (or ought?) to add your sheet entries to a top level schematic (and also use Sheet Entries on both sheets).

An advantage of using ports is that you can add an automatic label next to each port that shows where it connects to (Reports -> Port Cross Reference)

\$\endgroup\$
9
  • \$\begingroup\$ I think you're largely incorrect; the point of a Port is to traverse a hierarchical project, an off-sheet connector is declined to be used in flat designs. altium.com/documentation/altium-designer/… "Only supports horizontal connectivity (flat designs)" \$\endgroup\$
    – Chuck990
    Commented Dec 5, 2019 at 13:27
  • \$\begingroup\$ Huh, interesting, as that directly contradicts their own statements (linked in the answer). However, is there a reason you can't use ports on both sheets? (From your link: "Port - Used to connect a net from one schematic sheet to another. Connectivity can be vertical in a hierarchical design, or horizontal in a flat design") \$\endgroup\$
    – Araho
    Commented Dec 5, 2019 at 18:26
  • \$\begingroup\$ I can use either, but as a port produces the same error as the off-sheet connector, it's a bit of a moot point. \$\endgroup\$
    – Chuck990
    Commented Dec 6, 2019 at 9:29
  • \$\begingroup\$ Can you reproduce the error in a fresh project that you can share? I'm using the port -> port functionality in Altium right now, so it might be a project setting on your end? \$\endgroup\$
    – Araho
    Commented Dec 6, 2019 at 11:31
  • \$\begingroup\$ Sure, I've uploaded an example project with the bare minimum to show the issue - two sheets, one of which the net names used by the connector/port are also used by net labels. The compiler complains at both, calling them duplicate net names: we.tl/t-l5qG8ewSi3 \$\endgroup\$
    – Chuck990
    Commented Dec 6, 2019 at 13:33

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.