Copy components from a file to another

[Agrum]

Hello,
I have 2 pcb files (file A and file B) and I have to merge them in 1 file. I have selected and copied all components, tracks etc from file A and pasted in file B. It work but I have lost all net names.
It doesn't look a problem except the fact that if you want to make a track from the board B to the pasted board A you have to assign pad net in board A.
Do you think that this is ok or it's sound like a too rough method? Do you think that I'll lose some connections for some reasons?

Kind Regards

[ajb]

To do this right:

• In schematic preferences, make sure that "Reset Parts Designators On Paste" is disabled.
• Copy and paste the schematic elements from A to B--or if you're bringing over a whole schematic sheet, just copy and paste the file into your project directory and use "Add Existing to Project" from the project explorer.
• Copy the PCB elements from PCB A.
• Use "Paste Special" in PCB B, check "Keep Net Name", then click "Paste".
• Before doing anything else, from the menu in the PCB, select Project -> Component Links.
• Use the dialog to re-establish the links between the schematic components you've pasted in the schematics and the components you pasted into the PCB.
• Do a Sch -> PCB push to check for errors.
• Re-annotate your schematics if necessary to eliminate duplicate designators.  These changes should be able to be pushed from sch to pcb without issue.

[Agrum]

Thanks