Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
I´m new to Altium Designer. It seems like AD can´t use Off Sheet Connectors for hierarchical design, so I want to change all Off Sheet Connectors to Ports.
Is there an easy way to do this? Btw: There are a lot of Off Sheet Connectors in the design.
How can I use NetLabels in the hierarchical design? Somehow only Ports appear as Sheet Entries.
Thank you.
I would beg to differ with the answers posted here, but Altium absolutely has the ability to do what you're trying to do.
Because people sometimes use different names than others for the same thing, I'm just going to show a basic example, not necessarily tailored to your question, but you should be able to modify this easily to suit your needs.
The key to the solution is the Smart Paste tool.
Lets say I have a bunch of ports and I'd like to paste them onto nets of the same name. Simply select and Copy.
Click Edit -> Smart Paste
Here I chose paste as net labels and wires:
The final result:
As you can see from the second image, you can paste as Ports, Net Labels, even as Sheet entries where you can paste them onto a hierarchy.
This is very useful for connecting say a connector block up to a new hierarchy with a large number of nets. For example, from the same original Copied material, I pasted this onto a sheet symbol.
I trust you can modify this to suit your original question.
In Altium Designer ports are used to create sheet entries. Net labels are used to connect wires and buses inside a sheet only.
The power supply symbols (GND, VDD etc) are common over multiple sheets, so you don't need to make ports for them (although you can if you want it for clarity).
I don't think you can easily change the off-sheet connectors into a port, so you need to place a new port and give it the right name.
Altium documentation states the use of off-sheet symbols only for a specific reason:
Multiple sub-sheets may be referenced by a single sheet symbol. Separate each filename by a semi-colon in the Filename field. With the effective use of off-sheet connectors placed on the sub-sheets, you can effectively spread a section of your design over multiple sheets, treated as though they were one giant (flat) sheet. Note however, that use of off-sheet connectors is only possible for sheets referenced by the same sheet symbol.
If my memory serves, off-sheet connectors were really only included in Altium Designer for backwards-compatibility with older versions of the software (Protel). I generally use global net names instead.
As for changing off-sheet connectors to ports, I don't believe Altium currently has a good way to do that. I think you'd have to go through them one-by-one to replace them with ports. I ran into this a few months ago at work -- an old design used off-sheet symbols but we needed to change them to ports for use in a hierarchical schematic. We ended up having to go through and replacing them manually. It would be nice if Altium would allow the "Object Kind" to be changed in the Schematic Inspector.
EDIT: I tested Joel's answer and it works beautifully. Please disregard this answer.
