I have many net labels in schematics, now I want to rename some of them. But when I do, it doesn't update other net labels with same name.

Lets say I have 5 connection with 1 net label "Pin1", now I want to change it to "Pin5". Is there any way, that I change one and it updates all other 4. Yes there is Smart Edit replace, but that seems a trick and not a good way to do it.


3 Answers 3


Select the net label, right click on it, then select Find Similar Objects at the top of the list.

This window will appear: enter image description here

Select SAME for both Object Kind and Text. Now tick Select Matching at the bottom of the window and hit OK.

This action will highlight and select all net labels whose name is pin 1.

Press F11 to open up the SCH inspector and change the text from pin 1 to whatever you like.


You can use "Find Similar Objects" function with every type of object in Altium, even in the PCB Editor.

  • 1
    \$\begingroup\$ This only works for me when I also tick the Select Matching checkbox \$\endgroup\$ Nov 7, 2019 at 18:00

Ctrl+H is the search and replace dialog shortcut for Altium. Additionally, you can restrict the scope of the search to just net identifiers.

If you want to change 'Pin1' to 'Pin5', just use a simple text replacement.

If your concern is accidentally matching 'Pin11' in your search for 'Pin1', the "Whole word option" of the search (and search/replace) dialog is intended for exactly that purpose.

Alternatively, you can use the 'SCH List' panel to edit multiple items in parallel (right click, -> "Switch to Edit Mode"). It also has facilities for limiting the scope (set it to include only net labels).

  • \$\begingroup\$ yes but it could be problem if other net has pin1 in name too. I was thinking to have something like refactoring, where a dialogs pops and updates only specific connection, no matter what name is. \$\endgroup\$
    – xmen
    Mar 11, 2015 at 3:39
  • \$\begingroup\$ If you want to search for 'Pin1' and not 'Pin11', just check the 'Whole word only' checkbox. \$\endgroup\$ Mar 11, 2015 at 3:42

You can also use the SCH Filter tab from the Panels Menu.

Insert: StringText = 'TX' to find and select all labels and power ports with that name. Select scope current document or all documents to rename labels in more than one doc. Use SCH List to see the selected items. Select properties and change the name.

You can use (IsNetLabel) AND (StringText = 'TX') if you only want to select net labels or (IsPowerObject) for power objects. When using (StringText = 'TX') OR (Name = 'TX') then also ports should be selected.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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