Every SnapMagic download for Altium comes as its own schematic library (.SchLib) and PCB library (.PcbLib). If you already have company or project libraries, you can copy the symbol and footprint into them in a few minutes, so all your parts live in one place.
The screenshots below use Altium Designer 23. In the examples, 0ADBC2000-BE.SchLib and FUSE_0ADBC2000-BE.PcbLib are the SnapMagic download, and My_Company.SchLib and My_Company.PcbLib are the existing libraries.
Step 1: Copy the schematic symbol
Open both schematic libraries in Altium: the downloaded SchLib and your existing SchLib.
Switch to the downloaded SchLib. In the SCH Library panel, select the component, then go to Tools » Copy Component…
Select the part in the SCH Library panel, then choose Tools » Copy Component.
In the Destination Library dialog, select your existing SchLib and click OK.
Only libraries that are open in Altium appear in this list.
Switch to your existing SchLib. The part now appears in its SCH Library panel. Save the library with Ctrl+S.
The symbol is now part of your existing library.
Tip: You can also right-click the component in the SCH Library panel and choose Copy, then right-click in your existing library’s component list and choose Paste.
Step 2: Copy the footprint
Open both PCB libraries: the downloaded PcbLib and your existing PcbLib.
Switch to the downloaded PcbLib. In the PCB Library panel, right-click the footprint and choose Copy.
Right-click the footprint in the downloaded PcbLib and choose Copy.
Switch to your existing PcbLib. Right-click anywhere in the footprint list in the PCB Library panel and choose Paste 1 Components.
Right-click in your existing library’s footprint list and paste.
The footprint now appears in your existing PcbLib. Save the library with Ctrl+S.
The footprint is now part of your existing PCB library.
Step 3: Link the symbol to the footprint
This is the step that is easiest to miss. The symbol you copied still references a footprint, but Altium may not be able to find it now that the footprint lives in a different library.
In your existing SchLib, select the part. In the Editor area below the symbol, double-click the footprint model.
Double-click the footprint model to open the PCB Model dialog.
If the dialog says Footprint not found and the preview is empty, the link is broken.
A broken link: Altium can’t find the footprint.
Fix it under PCB Library:
Choose Library path, click Choose…, and select your existing PcbLib. Or:
Keep Any. This works only when your existing PcbLib is in the same library package or project as the SchLib, or is installed in the Components panel.
Make sure the Name field matches the footprint name in your PcbLib exactly. When the link works, the footprint appears under Selected Footprint. Click OK and save the SchLib.
Fixed: the footprint preview appears and “Found in” points to your existing library.
Step 4: Check all links with Model Manager
If you’ve added several parts, you can check every symbol-to-footprint link at once. In your SchLib, go to Tools » Model Manager… Select a component on the left. Its footprint and a preview appear on the right. If there’s no preview, that part’s link needs fixing.
Model Manager lists every component and shows whether its footprint is found.
What if my existing library is an IntLib?
An integrated library (.IntLib) is a compiled file, so you can’t add parts to it directly. Open the IntLib in Altium and choose Extract. Altium creates the source SchLib and PcbLib inside a library package (.LibPkg). Add your SnapMagic parts to those source libraries using the steps above, then right-click the library package in the Projects panel and choose Compile Integrated Library to build an updated IntLib.
Choose Extract to get editable source libraries.
Cleanup and other questions
Can I delete the downloaded libraries afterwards?
Yes, once the symbol and footprint are copied and linked. Close them in Altium first. Keeping them installed can lead to parts being placed from the wrong library by mistake.
I already placed the part on my schematic from the downloaded library. What now?
In your schematic, use Tools » Update From Libraries… to point placed parts at your existing library. Then run Design » Update PCB Document so the board picks up the change.
Still have questions?
If you have questions or feedback about a SnapMagic model, contact us at [email protected].