Create a new sheet from existing components wihtout losing placement?

[ajb]

I have an existing hierarchical design that has a few repeated channels, and after doing a fair bit of layout work it's become clear that I'm going to have to organize things a bit differently than I had originally planned so that everything will fit within mechanical constraints.  Ideally what is now a single sheet comprising the front and back ends of the repeated channel would be split into two sheets, one for the front end and one for the back end, so that I can separate them out on the PCB.  The trouble is, I can't figure out how to split the sheet up without breaking component links and losing the layout and routing work I've already done.  It seems like there ought to be a 'make new sheet from selected components' type of command, but if that exists I can't find it.  I can almost do it if I cut and paste from the existing sheet to a new sheet, manually update component links, and then update from schematic to PCB, but that's a pain and I can't quite seem to get it to work right.

Any suggestions?

[dboyer]

There is an option in the schematic editor settings to not reset designators upon copy/paste.  Could you cut, paste, and then automatically fix the component links based on designators?  That works without the hierarchical design, but I'm not sure how it will cooperate with your current setup.

[Rufus]

I would think if you make a copy of the .schdoc file and add it to the project all designators and unique IDs would be retained.  You could then delete the bits you don't need from each. Not sure what the implications of it being a repeated channel would be.

[ajb]

Okay, so I got it to work.  I already have Altium set to not reset designators on copy and paste, the trouble is that with repeated channels the automatically added suffixes aren't retained during copy and paste (because the editor view in the sheet for the repeated channel only has the base designator without the suffix)--so no matter what I can't see how to do it without breaking component links. 

So as far as I can tell, the way to do this is exactly what I was trying last night:  Move the desired components to the new sheet, manually repair component links (tedious, but relatively easy with suitable masks in the component link dialog as long as the base designators haven't changed), and then update from schematic to PCB.  The trouble I was having last night was that for some reason it takes multiple updates to get the component classes to synchronize properly and then it takes a couple rounds of online DRC to get the PCB editor to properly evaluate room placement.  So it's a bit of a headache, but at least it's doable, and I've got the schematic hierarchy to what I need without having to redo a bunch of layout work.

[ali80]

robert feranec from fedevel academy has a video showing exactly how to do it, just search through his videos