I'm pretty new to Altium Designer, so i hope you can help me.

While searching for some special components, I found some of them in the Vault database, but with the wrong footprints. That's why I'd like to convert them to a local Integrated Library, so I can rework them the way needed.

I know how to download the components to a Component Library (CmpLib) and how to find the footprints and symbols linked to it. But as they are on the Vault, I (of course) still can't rework them.

I already spent hours searching for a solution, but all i found were instructions to convert IntLib to CmpLib, not the other way round.

I hope you can help me!

  • \$\begingroup\$ This is a question that is relevant also for me. Have you had any progress in this? \$\endgroup\$ May 27, 2015 at 11:58

3 Answers 3


I did some more research on this. It seems like there is no easy way of converting a vault component into an Integrated Library. Easy way in the sense of for example right clicking a vault component and choose something like "Fetch current revision to local Integrated library".

There are ways within the Altium Vault window to find the schematic symbol and layout footprint. Look for the link within the preview section within each vault component. From there you can download the symbol and the footprint and put them together locally.

A better way (in my humble opinion) is to go to the Altium Design Content page. Here you will find all Altium Vault components available for download. Just find the library which contain the component you are looking for and download it. You will get a .zip file containing an .intlib file which can be extracted to a .schlib and a .pcblib. From there you can copy both the symbol and footprint into your own libraries.

  • \$\begingroup\$ Not sure how the "better way" would work. As an example, the Freescale MC33887 dual H-bridge is in the Altium content vault. However I can't seem to pull it up in the Altium design content page. Am I doing something stupid? \$\endgroup\$
    – akohlsmith
    Dec 2, 2015 at 7:37

I dont know if its because Altium updated their software, but now (AD16) there is an easy way to change the footprint of a vault component. Add your component from vault to the schematic. Then go to Tools->"Footprint Manager" and add an alternative footprint to your component. Then choose properties of your component and change the footprint.

Also there is now an option in vaults if you found a component, you can right click and download that component as CmpLib.


Starting with your local integrated library in AD18 and the Altium Content Vault part you want in the Explorer window:

  1. In Explorer, under the list of components is a list of the models in the component. Right click on the symbol you want and select Operations/Clone.
  2. The symbol you selected is now in a local library. You can edit this here if you like, but I prefer to right click on the Item ID and Copy. The I go to my schematic library and Paste.
  3. Edit the symbol (update the name, designator, clear out the parameter, ...) and save.
  4. Repeat for the footprint(s): Explorer, select footprint, Operations/Clone, Copy, Paste, Edit as needed, Save.
  5. Add the footprints to your schematic library model and make any other updates you'd like.
  6. Compile your local library and you are ready to use your local version of the Altium Content Vault part.
  7. You don't need the old, unedited/ unsaved clones of the parts anymore, so go to Projects, right click on the part (under Altium Content Vault, labeled "Copy of ...") and select Cancel Edit.

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.