The Vault components are intended for consumption only, not for modification, so creating a local library is not officially supported, and copied components will revert to their original form due to being updated with the original information from the vault.
However, this Knowledge Base article details how you may manually copy the vault components into your own components.
Procedure to convert Vault components to regular components
After the vault Symbol is copied to the schematic library it will still be mapped internally to the vault component and is also mapped to the footprint in the vault.
- You have a vault component placed in your schematic. Select the component and copy it to the clipboard.
- Open your SchLib library and focus the SCH Library panel
- Paste the schematic component into the library. This vault component will need to be rebuilt into a new component that is not linked to a vault.
- Double click the schematic component after pasting it into the library to show the Library Component Properties.
- Copy the contents of the Symbol Reference to the clipboard, then add a word to the end, e.g. DELETE, click OK in the dialog
- The vault component will now have a name ending in DELETE
- Click the Add button to create a new component, Ctrl+V to paste over the Component_1 text, press Enter to close the dialog and create the new component
- Paste into the filter field at the top with your Symbol Reference and notice only a few components are displayed
- Click on the Symbol Reference DELETE component and then click the Document Tab at the top of the editor window, to focus the editor
- Press Ctrl+A to select all, then click in the window to deselect, then Ctrl+A to select a second time (to work around a bug), then Ctrl+C to Copy
- Click on the new component, then click the Document Tab, Ctrl+V to Paste
- Double click the DELETE schematic component to show its properties
- Double click on the footprint model. Firstly, copy the text from the Name field to the clipboard, escape out of the dialogs.
- Double click the new schematic component to show its properties
- Double click on the footprint model.
- The PCB Library section will be set to Any. Change it to Library path and then click the Browse button at the top of the dialog. If necessary, select your PCB library that contains the footprint, then paste the footprint name into the Mask field. Click on the footprint in the list and click OK. This should populate the Library name field.
- Click OK and now the model is setup to use your own footprint library.
Top Comments