0
\$\begingroup\$

When doing schematic design in the Altium Designer, the Place menu contains these entries:

enter image description here

The 'Port' and 'Off Sheet Connector' can both be used to cross reference things on other pages of the schematic. This much is clear. However, I am trying to figure out these things:

  1. What is the difference between the two?
  2. How to know which one to use at a given time?
  3. Can't we just use net name from another sheet and they will still connect thus not needing the use of either of the above tools?

I have found that Altium Designer has a concept of hierarchical schematic design. However, I am not referring to that in this question. Maybe the above symbols are also used for hierarchical design, I am not sure.

\$\endgroup\$
1
  • \$\begingroup\$ I have never used the off-sheet connectors. I always use ports. But I vaguely remember that the off-sheet connectors caused lots of problems when I did try to use them long ago. I think maybe the off-sheet connectors are for hierarchical design, which I never do (and which I urge you also to never do unless you are part of a very large organization with very complex schematics and a lot of know-how about how to do it properly). Hopefully you will get a real answer. If not maybe this comment will lead you in the right direction. \$\endgroup\$
    – user57037
    Commented Mar 24, 2022 at 3:36

1 Answer 1

Reset to default
1
\$\begingroup\$

What is the difference between the two?

How to know which one to use at a given time?

They perform a similar function, and are both used to connect signals across different schematic sheets. The small difference is that Ports are intended to be used for hierarchical design, where you have child and parent sheets. Ports connect sheet symbols to sheets whereas off-sheet connectors cannot. Ports, like Nets, can be configured in the Net Identifier Scope from global to local, as you see fit to use in your design.

Can't we just use net name from another sheet and they will still connect thus not needing the use of either of the above tools?

Yes you can, if Net Identifier Scope is set to Global. It's your preference at the end of the day, but I do not personally recommend this.

I always use Ports whenever a Net needs to connect to a different sheet, never Off-sheet connectors. I find it helps me mentally comprehend the design space; I know that "Signal A" needs to travel via a certain place before arriving at it's final location, so it's essentially route planning, and I know where the stops are. When a design is being reviewed by a colleague, having a top sheet with ports shows the exact route I want the signals to go.

If your design with multiple sheets has only Net labels to describe the interconnections, then the reviewer must hunt down all of the locations of the Net label, with no idea of how many locations it has stopped at. This is tedious and allows errors to creep in.

\$\endgroup\$
2
  • \$\begingroup\$ When using ports, do different sheets have to be part of the same "design block" or "functional block"? \$\endgroup\$
    – quantum231
    Commented Mar 24, 2022 at 16:42
  • \$\begingroup\$ There is a tool in altium that automatically inserts page numbers at all the ports so you can see what page or pages also contain the same signal. This is one reason why ports are better than just letting nets get connected by name across schematic pages. This can also catch typos because every port should have a page number on it. If it doesn't then there is no matching port on any other page. \$\endgroup\$
    – user57037
    Commented Mar 26, 2022 at 3:23

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.