Create ports in Altium from (Excel) list

Question

Related, but does not answer my question: Is there a way to batch copy port names over to net names

I'm porting and updating a design into Altium. There are about 400 port names which needs to be handled. I have a complete list in Excel at the moment but I would very much like to not create them one by one by hand due to both time taken and risk of mistyping something.

Is there a way to create ports automatically from a list in Altium?

Internal design rules calls for ports and not a bus or harness, but I would be open to such solutions as well.

Answer 1

CTRL+SHIFT+V or Edit/Smart Paste:

Select Clipboard Contents from the bottom-left list. You can copy a list of (CRLF separated) text items from Notepad, Excel, SCH/PCB List panel, etc. and paste in the respective object type, which will inherit their StringText property from the clipboard contents.

Here I've gone to the SCH List panel, and copied the Text properties from the Off-Sheet Connectors. (Note that List and Inspector/Properties show this property as 'Text', but it is queried as 'StringText'.) Note that the list was unsorted, so the order has changed. (Remember to sort by Y1 value to preserve order from this source. Or other columns if you need a new ordering.) The new objects are created from object defaults.

Note that copying a compatible type (source in the top-left Object Type selection), transfers other compatible settings as well: color and orientation for example. Which may look out of place, but is easily corrected.