I have the layout for a 3.3V switching regulator module and I also made a 1.5V switching regulator module. The 3.3V layout is very nicely done and I would like to replicate it for the 1.5V. However, the 1.5V has a different schematic sheet and the components have different names (start with 1 instead of 3, e.g. R115 instead of R315.)

I used a snippet to duplicate my 3.3V schematic and then added it to a new sheet and changed the designators hoping that it would preserve my layout but it did not. My question is, how can I duplicate the 3.3V layout but use the 1.5V designators and connect it to my 1.5V schematic so that when I make a design change it will update the correct section?


This is building on this thread: Altium: reuse schematic AND pcb layout

I have no experience using snippets so any help is appreciated!


2 Answers 2



I don't think this is supported. Here's a workaround (hack):

1. Break the component links

From the Schematic,

Tools -->
Annotate Schematics... -->
Reset All -->
Update Changes List -->
Accept Changes (Create ECO) -->

When Altium reports the number changed, it should equal the number of parts in your schematic. If it won't do it for all parts, find the parts that keep re-annotating to the same ID/designator and manually reset those (double-click the part and click "Reset" next to the "Unique ID" field).

2. Perform a Design Update

Sync the changes over to the layout via the ECO system.

Altium will warn you that things don't match and allow you to match manually.

3. Fix the pours/tracks

If you have changed any net names, you will need to manually fix the affected pours and tracks. Altium will reset anything that no longer matches a netlist name to "No Net" so be careful to check for this or you will have a very fragile design that will cause you trouble later.


Assuming the naming difference is consistent, e.g. R10[x] is the same component as R30[x] and that I the two boards are based on the same PCB component models.

It is fairly easy to write a Delphi script or VB script to iterate through each component (sorted by ident) in both PCBs and copy the silkscreen attributes, text/font/size/location between them.

Script examples are inluded in your install and also available from the Altum Vault, these are a good starting point.


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.