how can I generate library from existing schematic?

Checking with the developers.

Wow, no answer yet?

For what it is worth:

I can select the components I want on the schematic and then copy them and then paste into a schematic library.  You can select multiple components at a time and copy and paste them.  If I select the entire schematic I can copy and paste into a new library.  The parts seem to be generated without error and any selected nets don't seem to bother the process.

Duplicated instances of parts will generate multiple components in the library.  So you would need to weed through duplicates.  This is actually probably safer than it trying to figure out what is and isn't truly a duplicate.  For example, you may have duplicate resistors but you changed the component properties.

CS has no ability to filter selections like AD does (with find similar components and masks).  That is a missing productivity feature they really should add to CS.

From the developers:

Thomas' answer is spot on. The SchLib file you've created will contain all of the symbols pasted from the schematic objects you copied. The wiring will be ignored when pasting.

The SCH Library panel has a field at the top that can be filtered to only show the duplicates, by typing *_ and then you can see the components ending in _# where # is a number. Other components with an underscore will also be displayed, so be careful not to delete them all without looking.

Footprints can be pasted the same way in your PcbLib file. The filtering is more accurate because you can use *duplicate and you're much less likely to accidentally delete a unique footprint.

Something to be aware of if copying from an existing schematic or PCB. If the original components were from the Altium Vault then you cannot successfully copy and edit them, the software will revert back to using the vault component and ultimately ignore any changes you try to make. If the components were from other sources then you should be able to copy and also modify as needed.

Did you know there are a huge number of component libraries available from the Altium design center? These can be downloaded, installed locally and then selected parts copied to local libraries and edited should you wish.

I can't seem to get this to work. I have the *.SchLib file open and am displaying the Library panel and schematic. I go to my schematic and select a component and choose "home->copy". When I go to the Library panel and right click it doesn't give me an option to paste new parts.

Thanks,

Brian

It is worth checking you are using the correct library panel. Open your schematic library and ensure View | Library is active (this is different to View | Libraries). Return to the schematic, copy your symbol and then select the library document again so that the library panel becomes visible. You should now be able to right click in the panel and Paste a new component.

Thank you! The wrong library panel got me again... I'ts now working as expected for schematic & layout footprints.

Brian