edit component in *.intlib library

Question

I have a previously used a resistor component in my project that originated from an *.intlib library.

Now I want to use an alternate footprint. However, I cannot access the .schlib file of the alternate resistor component in order to add the new footprint to the model.

What should I do?

Answer 1

Within Altium you will need to go to File -> Open and open the .intlib file:

Altium will ask you what you want to do, to which you should answer "Extract Sources":

This will generate a SchLib and PcbLib file, located under a "LibPkg" project:

Once you've finished the edits to your library files you can either re-compile as an IntLib, or you can keep the SchLib and PcbLib files separate (which is what I prefer to do, personally).

Answer 2

DerStrom8's approach is valid if you really want to edit the integrated library but there are a couple of other options which are often easier.

If you just want to change the footprint there is no real need to edit the library, you can change the footprint directly on the schematic and are not limited to one of the list the library author set.

• Double click the component to bring up it's properties.
• Select the footprint in the "models" section and hit the edit button.
• In the "PCB library" section of the dialog hit the "any" radio button.
• Enter the name of the footprint you want in the name box.
• Ok out.

Another useful technique is to use the "make schematic library" option in the schematic editor's design menu and the "make PCB library" option in the PCB editors design menu. These will build libraries from the components currently in use in your design.